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

Bestill vårt nyhetsbrev

autorisert forhandler av