Chat with us, powered by LiveChat

Tips

Thread Milling Operation for Mill/Turn

Edgecam Thread Milling Operation for Mill/Turn

The new Thread Milling operation is now available in the Mill/Turn environment, allowing more users to benefit from its advanced capabilities.

ec-tt-33--2.jpg

The operation can be used to machine wireframe and solid (associative) geometry, and offers support for helical arcs, canned cycles and integrated cutter radius compensation.

The operation has a graphical user interface, specifically designed to improve usability. On selecting a modifier an image or video explains the meaning of this parameter. Embedded help provides instant access to further information without the need to open an additional window.

The thread’s direction of cut depends on the values set for several parameters.

ec-tt-33-4.jpg

To support this Operation, a Threadmill tool type can filter threadmill tools in the toolstore. This can be specified in the toolchange (Milling Cutter dialog) or via the new ToolStore tool type.

ec-tt-32-3.jpg

Link til faq

Edgecam’s Improved Use of Instruction Browser

To improve the use of the Sequence Browser, Edgecam 2011 R1 now offers command context checking and cycle highlighting with changed features.

When working in Edgecam, manufacturing commands are grayed out until the correct mode or tool has been selected.

This can lead to problems when you move commands in the browser as you can inadvertently place a command where it would normally be unavailable.  When this happens, Edgecam now highlights the ‘out of context’ command with a purple background.  This allows you to rectify the problem.

Example:
The example below shows a Rotary/Planar Mode command that has been moved from its original position and that is now ‘out of context’ (the command is not available while turning).

ec-tt-32---3.jpg

ec-tt-32---4.jpg

Following a solids reload, features may change, which can affect the cycle using the features.

The Sequence Browser has been improved and any cycles that use a changed feature are now shown in red in the instruction list and flagged with a warning icon. This informs you that the input geometry to the cycle has changed and therefore may require some adjustment.

To clear the message, you need to accept the feature (right-click the feature in the Feature Browser and select Accept from the shortcut menu).  This can be done in Design mode.

ec-tt-32---2.jpg

Link til faq

Tech tips

Edgecam Tips & Tricks

The following is a list of Edgecam tips and tricks that you may or may not know:

•  Selecting the proper solid faces and/or entities can
be simplified by using the window command.
Depending on the direction the window is created,
can vary what faces and entities are selected.

o  Select a number of items by using click and drag to
enclose them in a window.

o  Left mouse click and drag from:

•  Left to right to select all entities that are within
the window created.

tech tip 30 -1.jpg

•  Right to left to select all entities that are within or
partially/intersecting the window created.

tech tip 30 -2.jpg

•  tech tip 30 -3.jpgClick Entity Types in the Input toolbar if you
want only certain types of entity to be selectable.

ec-tt-30-13.jpg

•  In the ‘Layers’ Tab, you can show this individual layer
by right clicking on the layer and selecting ‘Show
Only’.  Alternatively, you can right click in the ‘Layers’
Tab and ‘Show All’ layers.

•  tech tip 30 -5.jpgTo display features (in translucent form) click
Toggle Features in the Display toolbar to activate it.
Click Toggle Features again to de-activate it and
switch off the feature display.

tech tip 30 - 6.jpg

•  Choose between splitting the view horizontally or
vertically.

tech tip 30 - 7.jpg

•  To hide the toolpath for a specific instruction:

o  In the Sequence window, right-click on a
(machining) instruction.
A tick image-10.jpg  next to the option indicates that the
toolpath for the instruction is displayed.

o  Click the Visible option from the shortcut menu to
hide the toolpath for that instruction.
Hidden toolpaths are shown in pale grey in the
instruction list (see illustration, instruction 14).

tech tip 30 - 8.jpg

Note

•  You can hide the toolpath for an operation without
having to expand it.

•  You can select multiple instructions by holding down
the CTRL or SHIFT key while selecting the
instructions with a left mouse click.

Link til faq

Creating Stock

Creating Stock is an intricate process in setting up your component for manufacturing.

Stock is needed by Simulator, to show how the initial billet of material is being machined (if not already created, stock for Simulator can be automatically created on starting Simulator – you see a confirmation prompt).

Stock can be used by roughing cycles, so that the cycle knows where to remove material.  Use fixtures to represent how the work piece will be clamped to help avoid collisions. There are settings for avoiding fixtures in the Roughing cycle, for example.

Stock Notes

•    Stock is dynamic – it can be updated throughout
the sequence to show the effects of machining (so
roughing toolpaths can be adjusted accordingly). You
update usingM-Functions menu ►Update Stock.

•    The stock can be assigned to spindles on creating
a sequence.

•    Once created, you can assign the fixture as fixed,
or to an axis or spindle (dependent on the machine
capabilities). This is so that Simulator is aware of the
movement of the stock or fixture, so it can show any
collisions or gouges. (Note that for fixtures you then
need to use M-Functions menu ►Update Fixtures
so that the fixture is visible in Simulator).

•    Stock and Fixture items appear in the Features
window (Tree view).

•    Use Display toolbar ►Toggle Stock untitled-2.jpg to
switch between wireframe and translucent display of
stock and fixtures.

In Mill/Turn, the stock you see in Manufacture mode
depends on the tool selected. With a turn (static)
tool selected you see the ‘2D turn envelop’ stock.
With a milling (driven) tool selected, you see the 3D
stock.

•    When creating stock from a solid, the display
tolerance – which controls the faceting –  can affect
the size of the stock.

The dialog options are:

Automatic Stock   Check this to use the ‘Box Offset’ or
‘Cylinder Offset’ settings below to
define the stock.

Turn Envelope     This is only enabled in the Turn (ZX)
environment, and with ‘Shape’ set to
‘Digitize’ (below).

The geometry you digitize is
additionally used to form a ‘turn
envelope’ 2D turn stock outline. You
use this in the same way as a ‘Turn
Billet’ outline (see below).

The envelope represents the smallest
volume billet that you could machine
(turn) into the stock item.

The turn envelope and its solid body
stock are collected into a single item.
In mill/turning, you see the stock
represented by its turn envelope
(turn tool selected), or in its 3D form
(driven tool selected).

Type                      Select between Stock and Fixture.

Shape                   This setting determines how the
stock is derived.

        Box              You make two digitizes to define
opposite corners of the box. See
also ‘Depth’ below.

        Cylinder       You make two digitizes to define
the top and bottom extents of
the cylinder. See also ‘Radius’
below.

Profile         You digitize a 2D profile. See also
‘Depth’ below.  Edges and faces
should not cross over or exactly
meet as Simulator converts the
profile into a solid and this will
cause an illegal operation.  Use
‘Turn Billet’ in the Turn (ZX)
environment.

         Turn Billet  Generates 2D Turn stock from the
selected wireframe profile. This
option is typically used when
rough turning from casting or
forging to reduce air cutting and
to optimize cycle times.

The profile geometry must be
open.  The profile geometry need
not start and/or end on the
centerline; this is enforced
automatically.

           Digitize     You digitize a solid body or STL
model, which becomes the stock
item.  Although the geometry is
transferred to the Stock layer, it
is unaffected by this. In solid
bodies for example, you can still
find features or digitize the body
for machining. You control the
rendering of the solid using
Display toolbar ►Toggle Stock.
See also ‘Turn Envelope’ above.

Depth                   (Manual stock/fixture creation only)
Specifies the depth of the profile or
box stock/fixture. In Turn (ZX) this is
a Y depth. In Mill (XY) this is a Z
depth.

Radius                 (Manual stock/fixture creation only)
Specifies a radius of a cylindrical
stock/fixture.

Color                    The color of the stock or fixture.

Layer                    The layer the stock or fixture is to be
placed on. This is automatically set
to Stock or Fixture to match the
‘Type’ setting, but you can override
this and specify another existing
layer (select from the drop-down
list) or a new layer (type). Your
override setting is remembered and
not replaced by the Type setting;
reset Layer to Stock or Fixture to
revert to automatic settings.

Style                     The style for the lines of the stock or
fixture outline (Solid, Dotted and so
on).

Box Offset 

X/Y/Z Min/Max       (Automatic stock creation only)
These fields allow you to add
offsets to the stock. A positive
value will enlarge the bounding box
irrespective of its position relative
to the CPL. Offsets are incremental
and not absolute.

Cylinder Offset 

Start/End Extension   (Automatic stock creation only)
Allows the length at either end of
the cylinder stock to be extended.

Radius Extension     (Automatic stock creation only)
Allows the radius of the cylinder
stock to be extended.

untitled-4.jpg

Link til faq

Preparing Solid Models for Manufacturing - Automatic Feature Finding Part 4

Continuing on from the past Automatic Feature Finding Tech Tips, Select the Feature Find command, check the appropriate parameters and features in Feature Find dialog, select OK and Edgecam will interrogate the native solid model.  When the AFR has finished searching the solid model for features the Feedback window will be populated detailing what features have been found on the active CPL.

The Features Window

All features that are found using the AFR are listed in the Feature Window under the CPL in which they were located.

Using the Features Window, edit one of the Features by either image8.jpg  double left clicking or image9.jpgright click and Edit.

The dialogue box will differ depending on which type of feature you edit. The dialogue shown below represents a Hole Feature. It is possible to manually assign tapping data to the feature that can then be passed through to the Operations in Manufacturing. You can also edit the Geometry of the Feature.  Activating Preserve Depth will preserve the absolute Depth when altering the Level of a feature. This is because the Depth is relative to the Level, and if the Level is modified, the Depth moves with it by default.

All attributes of the feature can be viewed via the Properties window by highlighting the specific feature in the Features Window and selecting the Properties Window.

Toggle the render icon so that the solid model is shown in wireframe. Render the features using the Toggle Features icon found on the Display toolbar. This will render the features the same colors you specified in the Feature Finder dialogue box.

Toggle Features shown Translucent:

It may help you view the different features by switching layers off in the Layers window.


Link til faq

Preparing Solid Models for Manufacturing - Automatic Feature Finding Part 2

Feature Finding is a key element when preparing your solid model for Manufacturing.  These next steps will review the Features for Milling:

Features are named entities, or groups of entities, that you can select for machining. A feature might represent a pocket or boss for example.

  • Highest Wall Level ­– When identifying a pocket, the level of the pocket is raised to the highest point on the wall of the pocket. Use this option if you have a pocket within a pocket or the pocket is embedded in a complicated surface. See below:

solidmodels2.jpg

  • Un-checked
  • Checked

Feature Capping

  • TheFeature Caps option allows you to cover pocket or hole features in solid models with STL caps that can be used to exclude the hole or pocket feature from any surface machining cycle. To do this, the cap must be included in the cycle.
  • If the either of the Feature Caps option is checked when using the Feature Finder command on a solid with Find Pockets and/or Find Holes checked all pocket and/or hole features will be capped.

The following rules apply:

  • The caps are generated from the parent feature and are associative with the solid. Caps have their own definable layer, color and name.
  • Caps are represented as Edgecam STL entities and capped features are treated as STL models for surface machining instructions. If you explode a capped feature, the cap will be kept as a separate STL entity. Please note that exploding caps will break Associativity.

Holes

  • Find Vertical – Check this to find Holes that are parallel to the Z axis of their CPL.
  • Maximum Hole Diameter– Specifies the maximum diameter of a hole. Holes above this diameter will be recognized as a pocket not a hole, but below this diameter they will only be recognized as a hole feature.
  • Highest Concentric Level– If checked, concentric holes of the same radius at different heights will be found as one feature, that ranges in height from the bottom of the lowest hole to the top of the highest hole. If unchecked, concentric holes of the same radius at different heights will be found as separate features.
  • Thread Information– If checked this will assign thread information to hole features that had been passed from the CAD package.
  • Group Similar Holes– Check this box to group all holes with identical attributes.

Find Radial
Radial holes can be found if their axis intersects one of the axes of their CPL, as set by the axis property.

Find All Holes
New CPLs are created for the hole to be found, Hole_Find.1Hole_Find.2 and so on. (If an existing CPL cannot be used) This saves you from the laborious process of creating CPLs for the holes manually.

Mill

  • 2D/3D/Contour Pockets– The AFR will look for and record any Pockets on the solid model.
  • 2D/3D/Contour Bosses– The AFR will look for and record any Bosses on the solid model.

Contouring is making the sides of the feature more complex than simple vertical walls; for example by  taking a chain of lines and/or arcs and using this to represent part of the cross sectional profile through the feature. There are options for contouring in the Profiling cycle dialogue (Contouring tab), for example.

  • 3D Pocket/3D Boss– Check this to find features not falling into the previous two categories (2D and Contour); that is features with a free form shape. Note that the feature must have a single planar top face (bosses) or base (pockets) to be found (this is automatically the case for the 2D and Contour options).

Nesting

There is a Nesting option in the Feature Finder dialogue that you can set to:

Single – Pockets features found with this setting have a Nesting status property of Single, and cannot have bosses within them (even if the region of the solid model they are originally derived from does).

Nested – Pockets found with this setting have a Nesting status property of Nested, and can have bosses within them. Use this setting if you will be roughing out pockets with bosses, to prevent the boss being machined away.

Both – There are two coincident versions of every pocket feature; a Single and a Nested version.

Open Pocket

Check this for Open Pocket feature types to be found. Open pockets allow roughing without ramping (for example), as the tool can approach through the wall gap.

Open Mill

Check this for Open Mill feature types to be found. Open mill features allow roughing without ramping (for example), as the tool can approach through the wall gap as with Open Pockets. These will support multiple open sides, continuous draft angles, upper and Lower Radii.

Flat Face Features

Machining flat areas is now easier and safer using the new Flat Face feature type.

Use these, rather than the old Face feature type, for these benefits:

  • Can be automatically found along with other feature types using the Feature Finder command (new checkbox option for Flat Face features in the Mill tab).
  • Supports Strategy based machining.
  • Additional properties to help in tool selection and gouge avoidance (such as Neighbour (Yes/No) and Outside Diameter).
  • Associative to model.
  • Machine with FacemillFlat Land Finishing and Roughing cycles.

Notes on gouge protection: If there is any adjoining higher geometry in the solid, Facemill detects this and warns that it will not generate. Instead use Flat Land Finishing as this automatically machines round the geometry.

Link til faq

Preparing Solid Models for Manufacturing - Automatic Feature Finding Part 3

Preparing Solid Models for Manufacturing – Automatic Feature Finding Part 3

Feature Finding is a key element when preparing your solid model for Manufacturing.  These next steps will review the Features for Turning:

Features are named entities, or groups of entities, that you can select for machining. A feature might represent a pocket or boss for example.

The Turn Features options available are indicated below


Turn Feature

Set Start The Start of a Turn feature is the ‘highest Z’ end.

Front Face Minimum X The Front Turn feature starts at the point on the full envelope which has the maximum Z value, or if there are multiple such points, the one with the lowest X value.

Front Face Maximum X  The Front Turn feature starts at the point on the full envelope which has the maximum Z value, or if there are multiple  such points, the one with the highest X value.


Front Face Centreline The Front Turn feature starts at the point where Z = the maximum Z value of the full envelope, and X=0 (this may mean the feature profile loses contact with the solid).

Set End

The End of a Turn feature is the ‘lowest Z’ end.

None The Front Turn feature ends at the point on the full envelope which has the lowest Z value, or if there are multiple such points, the one with the highest X value.

Note that this setting produces an overlap in the Front Turn and Back Turn features.

Maximum X Start The Front Turn feature ends at the point on the full envelope which has the maximum X value, or if there are multiple such points, the one with the highest Z value.

Maximum X End The Front Turn feature ends at the point on the full envelope which has the maximum X value, or if there are multiple such points, the one with the lowest Z value.

Termination Z Set Termination Z (below) to a Z value at which to end the Front (and Back) Turn features.

Termination Z See the Termination Z setting for ‘Set End’ above.

Bore Features
Check this to find Front Bore and Back Bore features.

Set Start The ‘Start’ of a Turn feature is the ‘highest Z’ end.

Front Face Minimum X The Front Bore feature starts at the point on the full envelope which has the maximum Z value, or if there are multiple such points, the one with the lowest X value.

Front Face Maximum X The Front Bore feature starts at the point on the full envelope which has the maximum Z value, or if there are multiple such points, the one with the lowest X value.

Set End the End of a Turn feature is the ‘lowest Z’ end.

None The Front Bore feature ends at the point on the full envelope which has the lowest Z value, or if there are multiple such points, the one with the lowest X value.

Minimum X Start The Front Bore feature ends at the point on the full envelope which has the minimum X value, or if there are multiple such points, the one with the highest Z value.

Maximum X End The Front Bore feature ends at the point on the full envelope which has the minimum X value, or if there are multiple  such points, the one with the lowest Z value.

Termination Z Set ‘Termination Z’ (below) to a Z value at which to end the Front (and Back) Bore features (similar to the same ‘Set End’ option for ‘Turn’, above).

Termination Z See the ‘Termination Z’ setting for ‘Set End’ above.

Minimum Diameter No Bore features are found if they would have a diameter less than this.

Grooves 
Check this to find Groove features of all the various types (Front Turn Groove, Front Bore Groove and so on).

Threads
Check this to find Thread features. These can only be found from Part Modeler or Autodesk Inventor models.

Face Features
Front Face Check this to find the Front Face feature. This is the radial (parallel to X) portion of the full envelope that has the highest Z value.

image-6.jpgFront Face Minimum X  The Front Turn feature starts at the point on the full envelope which has the maximum Z value, or if there are multiple such points, the one with the Highest X value and finishes at the lowest X Value

Front Face Centreline As above but finishes at X=0 (this may mean the feature profile loses contact with the solid).

Back Face Check this to find the Back Face feature. This is the radial (parallel to X) portion of the full envelope that has the lowest Z value.

Back Face Minimum X and Back Face Centreline as Front face

Link til faq

Preparing Solid Models for Manufacturing - Automatic Feature Finding Part 1

Preparing Solid Models for Manufacturing – Automatic Feature Finding Part 1

Feature Finding is a key element when preparing your solid model for Manufacturing.  You can create features by:

  • automatically deriving them using the Feature Finder command
  • create them manually by specifying the key areas from which to derive the feature, using the Mill Feature command

Edgecam interrogates the solid model and features are derived from key areas in the solid, such as edges and faces, so they correspond to these areas. The correspondence is associative, so if the model is edited the Features automatically adapt themselves.

Feature Types (AFR)
The Feature Finder icon is located on the Solids toolbar, and can also be found under the Solids/Feature Findermenu from the Main toolbar.

When working with Solid Stock Bodies Edgecam can ignore these for feature finding, and automatically select a non-stock or Fixture body. This eliminates a digitise.

For this functionality in the XY Milling Environment, use the Auto setting of the new Component Selection option.  If you wish to feature find on the stock body, use the Digitise option.

Only the features in your specified CPLs are found. For example if some pocket geometry in the solid has a planar base parallel to the XY plane of the Top CPL, this would be found if you selected the Top CPL.

The CPL in which the feature was found is indicated by the feature’s ‘CPL’ property. The Feature Browser can show features grouped according their CPL.

You can also digitise faces in which to find features. This will automatically create a new CPL for the features (if necessary), based on the face orientation.

In the ZX Turning Environment, you will notice there are appropriate parameters in the Feature Finder.

Note:

  • This command is only available when a solid model is loaded.
  • Sometimes multiple features (duplicates) can be found at the same physical location, see this information on deleting duplicates.
  • By default, features are placed on a layer associated to the feature type and given a default color. You can use the Display tab to specify a color and layer for the found features.
  •  You can also feature find on a body in the current  CPL by right-clicking the solid in the Features Window and selecting the Feature Find option from the shortcut menu.

Link til faq

Creating Tabbed Views

Creating Tabbed Views will help orientate your component to custom work offsets to better view the components features.

The GLview is the standard way of viewing your part in Edgecam.  You can have one or more GLviews open in the Graphics Area.  Each looks at the part from a particular viewpoint, hence the view names of ‘Top’, ‘Isometric’ and so on.

A GLview appears like this:

The status bar at the bottom left shows the name of the view (Top) and the zoom magnification factor (5.07 in this case).   Left click or  Right click on the Status Bar and select New View…, from the pop up menu.

This dialog allows you to configure the view, create user defined tabs for tabbed views, control the layer options for a view and restrict the display of entities to a specified level by clipping views.

Edgecam has the ability to track the active CPL.

The new view will be displayed to the right of the Status Bar and a Default view will also be created.  The Default view uses the Edgecam default view settings.  With the Tracker view active and in Design mode, changing the active CPL will change the displayed view.  You have the ability to Pan & Zoom the part when a tabbed view is selected, but not Rotate. The tabbed view locks the orientation of the part so it cannot be accidentally changed. Select the Default view and the part can then be rotated as normal.

New views can also be created where views are aligned to a specific CPL.  Create a new view and select the appropriate CPL to align to.

It is good practice to meaningfully name the tabbed views you create. This will allow you to easily navigate around complex parts when creating machining instructions.  Use the other parameters in the Configure View dialogue box to specify display settings such as rendering, or translucency. These properties are specific to each individual tabbed view.

Link til faq

Align Body for Milling

The Align Body for Milling command will re-align and position a solid body for milling in this single command.

In cases where the imported solid component orientation is incorrect or if the CPL is not in the proper location, using the Align Body for Milling command will rotate a solid body to a more convenient orientation relative to the current CPL, and optionally move the body to a more convenient position within the CPL.

alignbodyformilling1.jpg

•    The command prompts you to digitize a face, edge and point, to be used for the re-orientation.
•    Each digitize immediately results in the re-orientation, so you can work interactively.
•    Perform a finish (right-click for example) to move on to the next prompt.
•   Before the finish you can digitize again to change your selection.
•   Before the finish you can digitize the same face or edge to rotate the body (see below).
•   You can perform the finish without digitizing if you want to skip a stage.

The prompts for alignbodyformilling2.jpg Align Body for Milling are:

1.    Select face to define XY plane

Click on a face to provide a vector to be aligned with the CPL’s Z Axis (face normal vector for planar faces, face axis for cylindrical, conical or toroidal faces). Click the face again if you want to then invert the body (rotates 180° around the Y Axis).

alignbodyformilling3.jpg

2.    Select linear edge to define CPL plane axis

Click on the edge that you want to be parallel with the CPL’s X Axis. Click the edge again if you want to rotate the body 90° around the CPL’s Z Axis.

alignbodyformilling4.jpg

3.    Select point to translate to origin

Click on the point you want to move to the CPL’s origin.

Alternatively you can position the centre of the solid at the origin (‘centre’ meaning the centre point of a bounding box round the solid). To do this hold down the Ctrl key and digitize the whole solid body, or any of its faces.

Before finishing you can optionally adjust the height of the solid by pressing the Z key, clicking OK in the co-ordinate dialog, then digitizing a point to be placed at Z=0.

alignbodyformilling5.jpg

Link til faq

Batch Mode

Emailing Large Edgecam Parts?

When e-mailing large Edgecam part files(.ppf) you can significantly reduce the file size by activating “Batch” mode. Simply make your very last CAM instruction “Batch Mode-On”. The CAM elements of the file will be reduced. Do however, remember to inform the recipient of the file to turn OFF batch mode upon opening the file.

 

Link til faq

Creating CPL's using Solid Models

Edgecam has the capability of creating a CPL from a solid face.

The CPL from Face command allows you to create a CPL from a solid face. This requires the selection of a face, plus an origin (optional). You can select the origin from any points on the model (including typed in co-ordinates and vertices). This CPL can then be used as a reference for machining purposes.

This function provides a method of CPL creation for Multi-plane applications. The full functionality for CPL creation is available through the normal Create CPL command, although this will first require you to create the Edgecam geometry.

Origin Check this box to specify an origin for the CPL which can be selected from vertices or any other defined points (including typed in co-ordinates).

Name Applies a name to the new CPL, if required.

Plane Specifies a method for redefining the plane of the CPL. Choose between the following options:

Face NormalAllows you to select a planar face from a solid for CPL creation.

Face Axis Allows you to select conical and cylindrical faces from a solid for CPL creation, typically useful in the multiplane milling environment when creating a CPL which is normal to a hole. The orientation is taken from the cylinder, the Z-axis of the CPL will point away from the middle of the cylinder. If the datum position for the CPL is above the centre of the cylinder the CPL’s Z axis will point up and if the datum is below the centre of the cylinder the Z axis will point down.

You will be prompted to pick the cylindrical face to define the CPL orientation.

You can intellisnap the origin at either end of the cylindrical face along the centreline of the cylinder. (This selection mode is optional and can be controlled by checking the appropriate box on the Selection tab of the Preferences (Options menu) dialog.
The default setting for this option is ON.)

Link til faq

Background Processing

Tired of waiting to process a large toolpath?

Edgecam introduces the ability to process more than one cycle at a time. This allows you to create and edit instructions in the foreground while other toolpath are still calculating in the background, significantly improving productivity. Background processing works on any hardware but offers the greatest benefits on multi-core PCs.
For improved feedback, the progress bar is integrated into the Instructions Browser for background processing. Cycles being processed are highlighted in yellow and progress is shown in green. If a process cannot start because it is waiting for all processes to finish (for example ‘Update Stock’) or because the maximum number of processes has been reached, this is indicated in the browser by a pale red background.

Please note that background processing is currently available in the milling environment.  Current supported cycles are: Roughing, Parallel Lace, Profiling, 5-Axis, Constant Cusp Finishing, Flat Land Finishing, Rest Finishing, Pencil Milling and the Projection cycles.

To process more than one cycle at a time, cycles need to know where to start and end independently of each other. For this purpose, Edgecam introduces a new command, Set Safe Start Position. When set, Edgecam knows it can process cycles in parallel. Note that this command needs to be disabled if you require cycles to start relative to the previous cycle. The Safe Start Position is indicated on the screen by a cyan dot.

You use this command to specify a point where each cycle (following the Set Safe Start Position instruction in the browser) will start and finish.  The Set Safe Start Position can be found under the Move menu ►  Set Safe Start Position

The Set Safe Start Position command is used:

•    To activate background processing. To process more than one cycle at a time, cycles need to know where to start and end independently of each other.  When a safe start position is set, Edgecam knows it can process cycles in parallel.
•    To reduce unnecessary cycle regenerations. Changing one cycle can alter the start point of the next cycle, causing a regeneration. This can cascade through the entire sequence, with all cycles being regenerated. By adding a safe start position, each cycle knows where it will start and finish. Regenerating one cycle will not affect subsequent cycles, reducing unnecessary regenerations.

To disable the safe start position

You may want to disable the safe start position, for example
•    if you require cycles to start relative to the previous cycle
•    to use toolpath optimization, such as ‘Nearest Neighbor’ in the Profiling cycle
To do this, you use the Move menu ► Disable Safe Start Position  command

Setting Preferences for Background Processing

To set the preferences, you use the Background Processing options (Options menu ► Preferences ► Toolpaths tab).

Maximum Number of Processes specifies the maximum number of instructions that can be processed simultaneously.  When that number is reached the subsequent cycles will not start processing until one of the existing processes has finished.

When running more than one process at the same time, there is a need for the computer to decide what tasks should get attention and be processed. You effectively use Process Priority to ‘rank’ the importance of background tasks.

Stopping a Background Process Cycle

As several cycles can be calculating at the same time the normal Abort command (F8) does not apply when using background processing. To stop a cycle that is currently being processed or has not started yet, right-click on the instruction to open the shortcut menu and select Stop. This will abort the calculation and turn the instruction red to indicate it has not completed

Available in Edgecam 2010 R2.


Link til faq

Hvordan gjemme verktøybanene for en maskineringssyklus (Visible, Axes, NC Code Output):

•    I Instructions-treet, høyreklikk på en maskineringssyklus. En hake  indikerer at verktøybanene for instruksjonen vises.

•    Ved å slå av Visible på en instruksjon, vises ikke verktøybanene for valgt instruksjon. Gjemte intruksjoner, vises utgrået i intruksjonstreet(se illustrasjonen, intruksjon 14).

•    Ønskes lenger akser på CPL, kan en høyreklikke på CPL-navn, nederst til venstre og velge Properties. Kryss av Axes-boksen og velg Ok.

•    Er det tilfeller der du ikke ønsker å poste ut NC-kode for en eller flere intruksjoner, har en muligheten til å bruke M-funksjonen NC Code Output der man har valg for å slå av ok på posting. command can either Suspend or Resume code output.

Link til faq

Thread Milling

Did you know that the Thread Milling cycle can reference feature properties?

Edgecam 2010 R1 introduces a New Thread Milling cycle. This combines features of profiling and hole cycle to overcome the limitations of the earlier cycle and to be compatible with other Edgecam instructions.
The cycle can be used to machine wireframe and solid (associative) geometry, and offers support for helical arcs, canned cycles and integrated cutter radius compensation, as well as simplified lead moves.

On the Thread tab, use ‘Associative’ and all thread parameters are taken from the feature in preference to dialog settings, unless a parameter is not set in the feature, in which case the value in the dialog is used.
If unchecked, the dialog settings are used in preference to the feature values.  Only available with ‘Model Type’ (General tab) set to ‘Solid’.

To support this cycle, Edgecam 2010 R1 introduces a new Threadmill tool type. This can be specified in the toolchange (Milling Cutter dialog) or via the new ToolStore tool type.

The new Thread Milling cycle (introduced in 2010 R1) has been further enhanced in Edgecam 2010 R2.  The cycle is now available in the Mill/Turn environment, allowing more users to benefit from its advanced capabilities.

Code Generator and Code Wizard enhancements ensure that templates fully support this functionality.

Link til faq

Using the Rationalise Command

Did you know you can re-order the instructions in the active milling sequence using the Rationalize command?

In the milling environment, you use the Rationalize dialog to re-order the instructions in the active sequence by ‘Tool’, ‘CPL’ or ‘Index’.

Before running the Rationalize command, you will need to set the ‘Sort Priority’ of the tools in the sequence.  The Sort Priority can be found on the ‘More’ tab when editing the tool.  Lower Sort Priorities are placed above higher values, so give toolchanges a value that will produce the correct order of machining, such as:

100 = Roughing
200 = Semi roughing
300 = Semi finishing
400 = Finishing
500 = Centre Drill / Spot face
600 = Drilling
700 = Tapping / Reaming / Boring

The Rationalize can be found in Instructions\Rationalize or you can access the command by right mouse clicking on the active sequence.

The dialog options are:

Strategy – Choose how you want to re-order the sequence:
•  By Tool – Reorders the sequence based on the toolchange instructions.  Instructions are moved in blocks that start with a toolchange instruction and extend to the instruction before the next toolchange.
o  The toolchanges (along with their ‘block’) are placed in order of their Sort Priority value. The lowest value is placed highest up the sequence.

A blank value is treated as ‘0’. If tools have the same Sort Priority, the sort on priority will group them together and their order within the group will be determined by their original (pre-rationalise) order.

o  All the repeat toolchange instructions (that is toolchanges back to the same tool) are then deleted. To be the ‘same tool’, all the toolchange parameters must match (Turret Position, Diameter, Offset and so on), as well as the Sort Priority setting.

•  By CPL – Reduces index moves by grouping together instructions that have:

o  The same rotary axis positions (as specified by Move menu ► Index). Any necessary retracts to safe distance are kept/inserted before the indexes.

o  The same datum (as specified by Move menu ► Index and/or M-Functions menu ► Datum Shift).

•  By Index – This produces the same result as by ‘By CPL’ above, except that the instructions datum is not taken into account.

Merge Hole Cycles – (Only available with Strategy set to ‘By Tool’)  Check this for the separate Hole cycles under a toolchange to be merged into one Hole cycle that machines all the holes.

Milling Safe Clearance – Retract moves to a safe clearance height may be inserted; before inserted index and datum shift instructions for example.  For these moves, specify how the safe Z value is to be derived:

•  Toolchange – The ‘Z Change’ parameter, as set in the Machine Parameters dialog, Tool Change tab

•  Max Clearance – The Maximum ‘Clearance’ value (as found in a Roughing cycle’s Depth tab, for example) of any of the instructions that are moved.
•  Z Initial – The ‘Initial Plane’ parameter, as set in the Machine Parameters dialog, General tab.

•  Safety Zone – Check this if you want to specify and ‘exclusion zone’, which determines the safe clearance height for the tool to retract to.  You use the ‘Safety Zone’ options (below) to specify the shape and extent of this zone.

Safety Zone – The Safety Zone options are only available with ‘Milling Safe Clearance’ set to ‘Safety Zone’.  Use these options to specify the shape and extent of an ‘exclusion zone’, which determines the safe clearance height for the tool to retract to.

•  Clearance Type – The shape of the safety zone.
o  None – No safety zone set.  If required, you will need to move the tool manually to a safe position.
o  Level – Safety clearances are referenced to a plane, relative to the Initial CPL. This is generally used when indexing and approach moves need to be above the component. Ideal for head/head and head/table machines where the tool can move above the component
o  Radius – Safety clearances are defined as a radius.  This option is generally used on  head/table machines. The tool will retract a radial distance from the centre of rotation or a specified CPL.
o  Sphere – Similar to the 5-Axis clearance type, safety clearances are referenced not to a ‘plane’ but a sphere

•  Distance – Specifies the extend of the safety zone.

•  Origin – (Only available with ‘Clearance Type’ set to ‘Radius’ or ‘Sphere’) Select a reference origin from a drop-down list. Please note that availability of this option is dependent on your machine configuration.

Link til faq

Corner Break in Finish Turn Cycle

Is your turning solid model missing chamfers and radii?

You can break the corners by setting the radius or chamfer value in the Finish Turn cycle. This has been improved in the Finish Turning cycle. The ‘Break’ corner type has been split into Break Chamfer and Break Radius, making it easier to specify either a radius or chamfer.

Other new options include Break Angle Threshold (to define which corners are chamfered) and Include First Entity (automatically applies the fillet/chamfer to the start of the profile – see illustration).

Corner Break options added to Finish Groove cycle

In addition, the corner break options have been added to the Corner Type selection in the Finish Groove cycle (Advanced tab).

Link til faq

ToolStore Administrator overview and how to backup your ToolStore

The ToolStore Administrator application is used to manage your ToolStore databases. It allows you to create new databases and backup, restore, and delete existing databases. The ToolStore databases can be stored on your local machine or hosted on a server, for access by client Edgecam machines.

You can also use ToolStore Administrator to switch the active database.  To copy a database to another installation (a colleague’s PC or a database-hosting server installation for example), you use ToolStore Administrator to create a backup of the database and then create a new ToolStore from this backup.

There can be a number of databases, but you only use one of these at any one time – this is the ‘active’ database. The currently active database is indicated by a blue tick. To change the active database, you follow the hyperlink in the top left of the dialog.

 Older databases that need to be upgraded before use in the current version of Edgecam are indicated by a red exclamation mark.

 When working in an older version of Edgecam, some databases may have a green exclamation mark. This indicates that the database is from a newer version of ToolStore and cannot be used.

For backing up your ToolStore databases, use Windows Start Menu ► All Programs ► Edgecam ► ToolStore Administrator . In the ToolStore Administrator, select ToolStore databases on the left.  Search the database for which ToolStore you wish to backup and left click on it.

Once you select the ToolStore, the next window will allow you to backup the database.

Select Backup Database, browse for a backup destination, give the database a file name and select the Backup button.

There are several ways of creating a new database, such as creating a new database from backup or an empty ToolStore.

 

Link til faq

PCI Templates

The template method populates a PCI file so that it can reproduce the current machining sequence. You can select specific instructions, with or without their dialog input. There is a single form-fill input for the variables used.

Use the Custom/PCI Template command.  You can only use this method in Manufacture Mode.

Note that you can also select the required commands in the Sequence Window. Then with a right mouse click, open the shortcut menu and select the PCI Template option.

The settings in this dialog are:

File Name For specifying the saved PCI path and filename. Type this in or use the Browse button.
Comments Use this to display a header/basic description before the initial user request at run-time.  This allows you to explain the purpose of the PCI and to tell the user which geometry elements to select. Use the Edit button to change the text.

 

After closing this dialog you will be presented with a list of the instructions in the current sequence. Pick the instructions to be included by selecting the individual instructions with a left mouse click.

•    To select a group of adjacent instructions, left-click on the name of the first instruction you want to include. Hold down the SHIFT key while selecting the last instruction with a left mouse click.
•    To select several non-adjacent instructions, left-click on the name of one instruction you want to include. Hold down the CTRL key while selecting each additional instruction with a left mouse click. This allows you to explain the purpose of the PCI and to tell the user which geometry elements to select.

After closing the dialog of instructions to add to your PCI, you will be displayed those instructions.  Here you can select which instructions to display when the PCI is ran.  For instance, you want to be able to change the ‘Cut Increment’ on both the Roughing cycles.  You would select both Rough instructions and the Rough Cycle dialog windows will be displayed when the PCI is ran.

Once you have completed the above steps, you can run your PCI from the Custom\Run Command File and browse for your PCI.

You can download short videos on creating PCI Templates below:

PCI Template for Milling

PCI Template for Turning

Link til faq

Rough Grooving Options

Below are options available in the Rough Groove Cycle that you may not be aware of.

Rapid Re-Approach
When using pecking in the Rough Grooving cycle, you can now opt for rapid approaches back to the material (rather than feedrate approaches), thus speeding up the cycle. To use this, check the new Rapid Re-Approach option on the Advanced tab.

There is a switch to the feedrate at your specified Re-Approach Safety distance from the material.

Peck Across
When using pecking in the Rough Grooving cycle, you can now opt for the ‘across the groove’ direction to have first priority over the plunge (tool axis) direction. This keeps the cuts more open, so easing swarf clearance.

You need to check the new Peck Across option (Advanced tab). Now, the tool will work across the groove, completing all the pecks down to a particular cutting (peck increment) depth, before returning to start of the groove and cutting down to the next peck increment depth (assuming a ‘Sequential’ cycle type setting).

Castellation Feedrate
Edgecam 2009 R2 saw the introduction of a new rough grooving strategy, Sequential Castellation.  The Rough Groove cycle has been enhanced further to allow you to specify a different feedrate for the second pass, removing the material left behind in the groove.

To use a different feedrate for the second pass, check the Castellation Feedrate option on the General tab.

*Note: These options are made available in Edgecam 2010 R1.

Link til faq

Saving MEG Files

You can now save .MEG (Machine Element Graphics) files directly.

MEG (Machine Element Graphics) files are used to save custom tool holder graphics.  Custom holder graphics can be added to a tool in the toolstore by browsing for the .meg file.  The MEG files are associative with the toolstore, so when the MEG file is updated because of a holder modification or update, the holder graphics in the toolstore will automatically update.

File menu ► Save MEG File command is used to save MEG (Machine Element Graphics) files directly.

This not only provides a quick way of saving a solid or STL to a MEG file, but also gives you the ability to automate the conversion to MEG format via a PCI script.  Load the solid model of your holder into Edgecam, locate the holder accordingly and select the Save MEG file.

Then move into the ToolStore and edit the tool to attach the holder to.  Move to the Mounting tab and Browse for the MEG file.

Link til faq

Stock Runout

Did you know the New Rough Turn cycle can move the turn tool off the part at an angle?

At the end of each cutting pass, the turn tool can be extended out towards the stock boundary at an angle. This removes any possibility of an undercut shoulder being left at the end of the cut.

Using the New Rough Turn cycle in Edgecam, on the Control Tab select “Stock Runout.”

Link til faq

Machining Either Side of Spindle

Edgecam allows you to machine on either side of the spindle centerline on a single turret lathe.

You may be working with a single turret machine that has the ability to machine on both sides of the spindle centerline. Edgecam creates turn features on either side of the component that can be selected to machine.

When selecting a Turning Tool, Edgecam offers a Centerline Side option on the General tab of the toolchange dialog.

*Note: These options are made available in Edgecam 2010 R1.  Adaptive post processors are required.

Link til faq

Finish Turn Cycle now has the ability to Use Current Stock

Following developments in Rough Turning in recent releases, the Use Current Stock option has been added to the Finish Turn cycle.  Use this option to restrict the toolpath to only those regions that have stock, without having to manually reposition the start/end arrows. This new functionality in effect adds a ‘rest machining’ capability to the Finish Turn cycle, and is also ideal for use with Strategy Manager to stop re-machining finished areas.  If required, you can apply Start/End extensions to each profile region. Normal Lead in and out moves will be applied all around the part.

To use this option, check the Use Current Stock parameter in the Finish Turning Cycle.

Notice in the image below, the highlighted toolpath shows the Finish Turning Cycle that has been created using the current stock.  You can see how it only machines the component where stock has been left from the previous cycles.

Link til faq

In Process Stock for Turning

In Process Stock is a new turning stock implementation within Edgecam. The basis of the stock is as before – a turn billet for example, but you use this stock in a different way, so that the stock:

•    Can be updated to show affects of machining on the stock.
•    Is always shown in Simulator (does not rely on Layer visibility).
•    Can be used dynamically in the New Rough Turn cycle, so that toolpaths are automatically updated with the affects of previous machining.

Stock needs to be created before the Manufacturing sequence has started.  Stock can be created automatically, from a solid, cylinder or from a turn billet.

Use the Auto setting for Initial Stock when you only have one stock item. Otherwise use <Digitise>, to manually select the stock (or <None> for no stock).

Note the new stock icon  in the Features Window (Tree view).

Create a New Rough Turn Cycle with the ‘Use Current Stock’ checked.

 Use the new M-Functions menu ► Update Stock command.

Note that this command only affects the new ‘In Process’ stock. You can convert the previous type of stock (with the icon   ) in existing parts by using M-Functions menu ► Lathe Setup, checking Select Stock, and digitizing the existing stock profile.

The Update Stock instruction ensures the toolpath is generated and dynamically adjusted according to the previous machining on the stock.

(Not available with an early ‘non-adaptive’ code generator selected.)

 

Link til faq

How to use a user variable for a list type modifier

Did you know that you can now use a user variable for a list type modifier?

In Strategy Manager, you have the option to insert a string user variable in a list type modifier (such as Tool Type where the list is Drill, End Mill, Ballnose, etc.)

The example below will select a tool either End Mill or Bullnose based upon the MinZRadius of the pocket being machined.

Previously you would have had to output one of several versions of the process, each having a different ‘hard coded’ setting.

Link til faq

In Process Stock for Milling

Did you know that Edgecam 2009 R2 now has In Process Stock for Milling?

The Roughing cycle can now use In Process (dynamic) stock in the milling environment.  When creating a Roughing Cycle, set the Stock Type to ‘Current Stock’.  The Stock Offset parameter will allow you to set a 3D offset amount that’s applied to the stock’s current state.  After generating a Roughing Cycle, use M-Functions menu ► Update Stock, to update the stock with the effects of previous machining.  If a second Roughing Cycle is created with Stock Type set to ‘Current Stock’, the cycle will now have a dynamic link to the stock, so it will adapt itself to any changes to the stock machining higher up the sequence.

Using the Update Stock command is useful for updating cycles using ‘Current Stock’, so that the toolpaths are updated accordingly to how the stock has been machined previously in the sequence.

As a reminder, In Process Stock for Turning was also made available in Edgecam 2009 R1.

Link til faq

How to use "Align Body for Turning" command

In cases where the imported solid component orientation is incorrect or if the CPL is not in the proper location, using the Align Body for Turning command will re-align and position the solid component for proper turning.

• The command prompts you to digitize faces to be used for the re-orientation.

• Each digitize immediately results in the re-orientation, so you can work interactively.

• Perform a finish to move on to the next prompt.
o Before the finish you can digitize again to change your selection.
o Before the finish you can digitize the same face or edge to rotate the body.
o You can perform the finish without digitizing if you want to skip a stage.

Select the Align Body for Turning command    and follow along with the prompts:

1. Select face to define axis of rotation
o Click on a cylindrical face to be aligned with and centered around the Z axis.  Click the face again if you want to then invert the body (rotates 180° around the X axis)

2. Select face to define origin plane
o Click on the face that you want to be placed at the origin (center of face placed at Z & X =0 )

3. Select face to define C orientation
o Click on a face that you want to be normal to the X axis, rotating the part around Z.  This will typically be a flat on a cylindrical face.  Each subsequent click further rotates the body 90° around Z.  As an alternative to a flat face, you can click one of the faces of a radial hole.

Note that you can also opt for the part to be automatically aligned on opening – check Options menu ► Preferences ► Solids tab ► Auto align for turn. You need the ZX environment set as the default, as determined by the specified defaults file.)

Align Body for Milling  command is also available to rotate a solid body to an orientation relative to the current CPL, and optionally move the body to a relative position within the CPL.

Link til faq

Intellisnap: What is it and how do you use it?

Intellisnap: What is it and how do you use it?

“Intellisnap” has multiple functions that you can take advantage of. When turned on, it will display a feedback window with information about entities. Right click in the Graphics Area of Edgecam and select ‘Intellisnap’.

Place the cursor over any entity and it will display the entity type and layer it’s on. Selecting the ‘V’ button on the keyboard will display additional information about the entity.

Where more than one entity is selectable in a given position (where two faces meet for example) you will see the symbol. You can use the ‘Tab’ key to toggle through the selections.

Also, when you are digitizing, Intellisnap automatically displays points on existing geometry such as mid-points, end points, intersections etc. As your cursor nears these points, they become highlighted and your click selects these points exactly.

 

In the Manufacturing Environment, place the cursor over a toolpath created. It will display which tool is used in the toolpath, cycle type, and also the cycle time.

Link til faq

Useful tips and tricks you may not know

Edgecam Tips and Tricks

The following is a list of Edgecam tips and tricks that you may or may not know: 

• To rotate the model around    , click and hold the right mouse button.
• To pan the model  click and hold the center mouse wheel.

• Zoom in and out by scrolling the center mouse wheel.

• Ctrl-E will fit the model in the screen.

• To rotate the model about a certain point, position the curser on a desired spot on the model.  While holding down the Ctrl key, right mouse click on the desired point.  Then click and hold the right mouse button to rotate normally.

• When rotating the model using the right mouse button, holding the X, Y, or Z button on the keyboard will fix the model to rotate around the designated axis only.

• Keyboard Hot Keys
o Zoom Extents – Ctrl E 
o Rotate View in X – Ctrl Up or Down
o Rotate View in Y – Ctrl Left or Right

• Standard views of the component can be selected by right clicking on the View Caption and selecting the desired view

• Just above the status bar is a CPL marker showing the orientation of the current CPL, as seen from the current view.  This marker shows the X axisY axis, and Z axis of the CPL.
o X axis – Red                              
o Y axis – Green
o Z axis – Blue

• To view larger axes than shown with the current CPL, right click on the View Caption and select Properties.  Check the Axes box and select Ok.

• Automatically align the component view with the current CPL by right clicking on the View Caption and checking Track CPL.

• To use the model color values from the native CAD system, go to Options, Preferences and on the Solids tab, uncheck Ignore Model Values.

• To change the model colors, right click on the model in the Feature window and select Edit.  You can then change the color and the layer the model is on.

• Make Simulate Machining window open Maximized.

Select the Simulate Machining command to start up Simulator.  Once opened, right click in the graphics area and select Options.  On the General Tab, select Maximized and click Ok.  Next time Simulator is opened, it will run full screen.

Link til faq

How to transfer features

Did you know that features can be transferred between the main spindle and sub spindle?

You are able to copy or move features between the main spindle and sub-spindle at will, using the new entries in the Features Window shortcut menu. You can use these to override the automatic spindle assignment, as determined by your ‘Mill Features Spindle Assignment’ settings, on creating the machining sequence.

For machines with both Main and Sub-spindles, features have “Copy to other spindle” and Move to other spindle” commands.  Right click on a feature to either copy or move the features from one spindle to the other.

Link til faq

How to park turrets during sub-spindle docking

Did you know that you can park turrets during sub-spindle docking?

The toolchange position is not necessarily a safe position for sub-spindle docking. 

In Edgecam 2009 R2, use the new Move menu Turret Parking  command to return the turret to a safe co-ordinate position and index station prior to sub-spindle docking.

Note that you need to insert any required Synchronize Turrets commands – these are not automatically inserted.

If a park instruction is not immediately followed by a move to toolchange on that same turret, you use the Turret Unpark command to generate a move to the toolchange position.

Turret Parking moves will be simulated in Edgecam Simulator.

Link til faq

Feature Find

Have you ever been in Manufacturing mode and noticed you missed a feature?

Feature Finding commands can now be run in Manufacture mode.  The appropriate commands can now be executed from the Solids menu and toolbar in Manufacture.

Also under the Solid menu, you can Accept  All Features that have been created in Manufacturing.  No need to move back to Design to accept the new features when revision changes occur and the model updates with new features.

Link til faq

Simulation Enhancements

Start Simulation from the first command every time?  

Not anymore….

Simulator has been enhanced in Edgecam 2012 R2 so that you can now start the simulation from any point in the instruction list.

Use the Sequence Browser (no available in Simulator) to start the simulation at any point by clicking the instruction in the list.  Rewind to any previous point in simulation without having to fast forward through each tool change.
There’s no need to simulate the whole sequence each time just to view a specific machining command or instruction.  Simply pick exactly which instruction to simulate.

Simulator also allows you to specify where to stop the simulation, by clicking the simulator toolbar Stop Options command and selecting the required options.  In Edgecam 2012 R2, Simulator has been enhanced for more control over where to stop the simulation

Several new options include Stop at Axis Overtravel, Stop at Stock Transfer and Stop at Next Sequence.

Link til faq

Edgecam 2013 R1 - Rough Profile Cycle in Turning

Edgecam 2013 R1 Releases a New Rough Profile Cycle in Turning.

The Rough Profiling cycle removes material in a series of cuts parallel to the input profile and is typically used for roughing free form profiles from free form stock billets. It is also useful for cutting materials where it is beneficial to minimize re-entrant cutting as it keeps the tool in contact with the material for longer.

Benefits of the new cycle include:

  • Stock aware to eliminate air cuts and reduce cycle time.
  • Intelligent stock entry and exit.
  • Support for controller tool offset i.e. G41/G42.
  • Constant cut depth or different cut depths for X and Z.
  • Specify ZX or Constant Offset finishing allowance.
  • Machining attributes

    *This new cycle replaces the old Rough Profile Cycle and is available in all Turning and Production licenses.

Link til faq

Automatic Feature Recognition

Automatic Feature Recognition is great and all, but sometimes it does not give me what I want.

Solution:  Create a Manual Feature

Manual Features can be created for either milling features or turning features, allowing the user to select what they want to include in that particular feature.

Learn More:

Under the Solids menu, select from Mill Features, Hole Features, and others to create your custom manual features.

Link til faq

Waveform Roughing Improvements in Edgecam 2013 R1

The Waveform strategy now has the option to set the Approach Type as Helix or Pre-Drill.  It works in the same way as other strategies where a 10% larger drill is expected for the pre-drill option.

The Plunge feedrate for approach moves can now be specified as a percentage of the Plunge feedrate
on the General tab. This option is available for all Roughing strategy types.

Some machines tools, due to the «Look Ahead» calculation and the high feeds, may leave pegs in the
material showing unmachined areas. These pegs would be removed if the feeds were reduced,
meaning that the toolpath is correct but, due to the «Look Ahead» calculation, the machine tool is
avoiding those areas. Clean Up Final Pass has been added to the Control options which will add a pass at the end of the area to ensure that all material has been removed.

Waveforms Roughing pattern has been improved to avoid unnecessary cutting interruptions when opening the initial ‘virtual pocket’.  The transition between this are and actual toolpath is much smoother.

Link til faq

Profiling Cycle – New Break Corner Options

he Profiling Cycle has been updated to include options to break sharp corners with either a radius or a chamfer.  This will help to reduce secondary de-burring operations.

Link til faq

New Rough Profile Cycle

This is a new cycle that replaces the Rough Profile cycle.  The Rough Profiling cycle removes material in a series of cuts parallel to the input profile and is typically used for roughing free form profiles from free form stock billets. It is also useful for cutting materials where it is beneficial to minimize re-entrant cutting as it keeps the tool in contact with the material for longer.

Benefits of the new cycle include:

  • Cycle is optionally stock aware to eliminate air cuts and reduce cycle time.
  • Intelligent stock entry and exit.
  • Support for controller tool offset i.e. G41/G42.
  • Possibility to enter a constant cut depth or different cut depths for X and Z.
  • Specify ZX or Constant Offset finishing allowance.
  • Possibility to enter different offsets for each face element.
  • Option to stop after a specified no. of cuts, return to a safe swarf clearance position, stop the machine, clear the swarf then carry on.

The old Rough Profile cycle has been removed from the default user interface, but can be retrieved using  Customize ->Commands -> Turn Cycles

Link til faq

Have you created the wrong size stock and need to edit the size?

If you created the wrong size stock or in the wrong location, there’s no need to delete and start over.  In Edgecam 2013 R1, a number of improvements have been made to the Design Stock command:

•    Ability to edit stocks and re-pick geometry or depth, retaining the original type
•    Profile Stocks now support hollow, holes, and through pockets.
•    Tube stocks for turning and milling.
•    Stock Profile can now be consistently created from a closed shape without rendering
problems
•    Arcs are no longer split into several segments of lines

Either right click on the Stock in the Features window or double click on the stock in the graphics area to edit.

Link til faq

Moving the Sub-Spindle - Option to Return Home Without the Part

The sub-spindle can be docked to support the part for a machining process after which it
may be sent back to its home position without the part. Previously, the stock was always returned home with the sub spindle.

Note:

If the With Part option is selected, the sub spindle should be docked at its final grip position prior to
returning home with the part. If it is not, a message is issued requesting you do this.

Link til faq

Endre innstillinger ifm auto-orientering og plassering av nullpunkt ved åpning av CAD-filer. (Workflow Alignment Options)

Når er åpner en del i Edgecam Workflow, vil delen automatisk åpnes i rett miljø (drei eller fres) og orienteres utfra forhåndsdefinert oppsett. Disse reglene kan endres ved å velge fanen File også Preferences.

Om en vil bruke CAD-filen sitt nullpunkt istedet, fjernes haken Align for Milling, hvis dette kun ønskes på fresedeler.

Link til faq

Endre rotasjonspunktet på modellen

En kan enkelt endre rotasjonspunktet som brukes når en roterer modellen. Hold nede Ctrl og høyreklikk på ønsket rotajonspunkt

Link til faq

Bestill vårt nyhetsbrev

autorisert forhandler av