CAD
Tips & Techniques 
Tips & Techniques are provided here and throughout the documentation. They provide useful information and guidance that can help you take full advantage of VX CAD and its many advanced features.
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The following icon is used to indicate those Tips & Techniques that are new to this page for the current VX release. They do not necessarily indicate new functionality.
Select from the following sections:
Make plenty of memory available for VX
VX
performs memory checks and alerts you if you do not have enough memory
or if you are running low on memory. The alert is made if you do not have
at least 768 MB of total memory (physical+virtual) when starting VX and
if you have less than 128 MB of total memory available while running VX.
If you see this alert, check to see if you have other applications running in the background and close them. This will avoid a possible system failure. VX and your system performance in general will benefit when you make plenty of memory available. See also VX System Requirements.
Keep an eye out for the Regenerate Current Part icon
Keep
an eye out for the Regenerate Current Part icon.
When it turns GREEN, that means that the parametric history of the current
part has been modified and needs to be regenerated. Save your file before
selecting the icon to regenerate. If errors occur during the regen due
to recent parametric edits you have made, then you can undo the regen
or load your most recent save.
Regenerate Current Part Icon
Read
the command prompt. It will prompt you for the
next input required. Also pay attention to the message window. It provides
command status and reports messages about the current operation. The message
window can be expanded to review previous messages.
CAUTION:If you delete an entity, all entities associated with that
entity will become disassociated. This
could cause unexpected results that may be difficult to correct if the
association is discovered much later or by another operator. Here
some entities to consider:
Root objects
Parts and assemblies can be associated with other assemblies as instanced components and referenced by layout views in a drawing sheet. Drawing sheets can occur as instances in other drawing packets.
Features
It is good practice to delete one feature at a time and perform a History Regen after each deletion to verify the integrity of the active part. If the part will not regen properly, Undo the last feature deleted. A successful regen will not occur if there are features dependent upon the deleted feature. You may have to delete the dependent features as well or you can try reordering features to isolate the feature you want to delete.
The active session - What to remember during advanced session management
To temporarily set the max undo/redo for the active session
You
can use a command line function to temporarily change the maximum number
of undo/redo steps that are logged during the active
session only. The syntax is "$NumUndo <number of steps>".
For example, to set the number of undo/redo steps to 100, in the text
input field you would type "$NumUndo 100" (quotes excluded).
This function will temporarily override the max undo/redo setting defined
in the VX Configuration Form for the active
session only.
Avoid having two VX files with the same name
CAUTION:You cannot activate
two files during the same session that have the same name but reside in
different directories. You have to clear the file edit already associated
with the active session with the Clear
File Edit command before you can open another
file with the same name. If you want to save any changes made to the file
during the active session use the Save
File command first.
Session management enables a collection of advanced VX functions designed to further manage user sessions. These functions can be found by selecting File > Manage Session but only when the "Enable session management?" option on the Files tab of the VX Configuration Form is enabled. Be sure to review Appendix C : Advanced Tools : Advanced Session Management before using these advanced functions. A few Tips & Techniques are provided below.
Backup Session (Ctrl+B) - Advanced session management function
Avoid saving the same file from multiple sessions
CAUTION:Avoid editing and saving
the same VX file from two or more different sessions. The sessions may
become out-of-sync with the file. Save the file
under a new name first and then access the new file in another session.
If there is a root object in a file that you want to access from another
session, you can move or copy
it to a new or existing file and then access it from the subsequent session.
Use
the Save File As command at various
stages in your design to save your progress under different names. You
may want to return to a previous stage in your design.
A quick jump to your user directory
VX
has a built-in VX PDM (Product Data Management)
system. Even
if you don't plan on using it, it provides a quick way to get back to
your user directory from the File
Browser. Select
Utilities > Configuration...
and go to the PDM Tab on in the
VX Configuration Form. In
the VX PDM section, set the Vault directory to an existing directory
(this turns VX PDM on) and set the Work
directory to your user directory and then
pick OK. Now,
anytime the File Browser is displayed, you can
select your user directory from the PDM drop-down list. VX defaults to
the last folder visited but this will jump you back to your user
directory in a snap!
Activating files and objects when starting VX
You
can activate a root object for editing when you start VX from the operating
system prompt. The syntax is:
vx -f<path and source file name> -o <root object name>
The "-o" argument may be excluded to simply activate a
file for editing.
Type vxv -h at the system prompt to display VX command line help.
VX Exchange Files - How they differs from the VX Neutral File
What you should know about importing geometry with dimensions into a sketch
Dimensions
will loose their associativity with base geometry when imported into a
sketch. Dimensions with no associated geometry are prevented from being
added to the solver. You can however, work on the geometry as you normally
would. Since the imported dimensions are not part of the constraint system
they will not change if the sketch geometry changes. If you want to have
dimensions move with the geometry, you will need to delete the imported
dimensions and recreate them in the sketcher.
VX
has predefined hundreds of standard hole attributes into a library called
"Bundles.VX" stored
in the "driver/resource"
folder of your User Directory.
These are standard holes based on the "Machinery's Hand Book" and include thread and tolerance values. These values are stored to the 6th decimal place to meet the standard.
Pick the folder icon on the Hole Feature Options Form and use the File Browser to locate the "Bundles.VX" file (if it's not already selected) and then select a hole from the drop-down list. The options form will populate with the selected hole's attributes.
You
can use the Clear Facets command from
the View Menu to clear all facet data (used for shaded display)
from the active part. The next time the part is displayed in shaded mode,
facet data will be regenerated. Deleting the facet data from a part before
saving it will reduce the size of the resultant file. This command is
not logged in the undo/redo history. Once executed, it cannot be undone.
This is more of a space (file size) saving tip than a time saver.
Defining the curve portion during the FEM Refit Curve command
Part Attributes - Using non-graphic components (e.g., paint, grease)
Original point data is not backed up in the active
parts history
When you should regenerate the part history
The
history of a part or assembly is very important to the part's integrity
and to all other parts and assemblies that reference it. There
are number of situations when regenerating the part
history is strongly recommended.
After editing
dimensions -You
should always perform a History Regen
after editing a dimension to verify the integrity of the active part.
If the modification causes an error in the part's topology, you may select
not to keep the changes and adjust the dimension modification accordingly.
If you postpone the history regen an error introduced now will be more
difficult to locate and correct.
After reordering
features - You can use the Cut, Copy
and Paste feature commands to reorder
features within the active part's history. Always perform a History Regen after reordering features
to verify the integrity of the active part. If the reordering causes an
error in the part's topology, you may select not to keep the changes and
adjust the new order accordingly. If you postpone the history regen an
error introduced now will be more difficult to locate and correct.
After suppressing
features - You should always
perform a History Regen after suppressing
features to verify the integrity of the active part. If an error in the
part's topology is introduced due to other features being dependent on
the suppressed feature, you may Undo the suppression. If you postpone
the History Regen, an error that is
introduced will be more difficult to locate and correct.
Incrementally after editing - You should always perform a History Regen incrementally after editing to verify the integrity of the active part. If the modification causes an error in the part's topology, you may select undo the changes and make adjustments accordingly. If you postpone the History Regen, an error introduced in an earlier edit will be more difficult to locate and correct.
If you get an error when displaying isolines on a face
In
some unique cases the isoline display data of an imported face may not
display properly. In this case, an error message is displayed and a label
"Face N" is shown for faces that cannot otherwise be displayed.
This allows them to be picked and deleted. This label is only shown in
wireframe mode.
What you should know about copying sketches
Copying
a sketch using any of the commands on the Edit
> Copy, Edit > Pattern
or Edit > Mirror commands will
result in a locked sketch. This means that the sketch copies will be locked
against "geometric" editing. The sketch can be parametrically
edited by modifying its dimensions (double-click
a dimension to edit it) but it cannot be loaded into the sketcher for
geometric editing.
Copying, patterning, or mirroring a sketch is used primarily in preparation for Loft commands where sketch copies with varying dimension values can be used.
There are also other ways to copy a sketch or its geometry. You can use the Copy Features to Clipboard command and then paste the sketch into the active part's history. You can also use the Cut to Clipboard command at the sketch level and then paste the geometry into another sketch or drawing sheet. A locked sketch can be used for any feature creation the same as a regular sketch.
Curve editing with parting lines
Parting
lines are curve features that behave differently from other wireframe
curves when they are edited. The Tools
> Mold & Die menu contains commands specifically designed
for editing parting lines.
Use caution
when modifying the geometry tolerance
CAUTION:Modifying the geometry
tolerance may cause a history regen to fail. It
is recommended that you perform a history regen
after modifying the geometry tolerance. If the change in tolerance causes
the regen to fail, you can undo the change. If you regenerate later, a
failure now may be more difficult to locate and correct.
Try to settle on a tolerance value that is right for the
size and complexity of the part before you begin a design. A tolerance
value that is too small will cause increased processing times and increase
the complexity and size of the model's database. A value that is too large
may cause the system to ignore features that are very small relative to
larger features and decrease the accuracy of intersections and curve/face
approximations.
The right tolerance value is one that is only small enough
to allow the accurate definition of the smallest anticipated feature and
the amount of geometric variation that can be tolerated.
What you should know about working in shaded display mode
CAUTION:The facets generated
when the Shaded Display mode is active are an approximate
representation of the actual part. Be aware, part features that are much
smaller in relation to the current View Extent value may be misrepresented
or removed from the shaded display altogether. Decreasing the View Extent
value (zooming in) and regenerating the display facets will increase the
total number of facets so that these features can be viewed more clearly.
When curves are too small to display
It
may be possible to have curves that are so small that they are not being
drawn and therefore, are not selectable (such as a result of imported
geometry). The display method for 3D wireframe curves has been upgraded
so that an asterisk "*" point marker is displayed for "tiny"
curves. This allows you to "see" and pick (e.g. for deletion)
these curves.
When defining base, boss and cut features
Try
to define base, boss and cut features so that they represent the final
shape of your part as much as possible. Doing so will minimize the number
of additional features required and will help minimize model size and
complexity.
Why you should assigning unique names to features
Assigning
your own unique name to a feature is better than accepting a system-generated
name. Assigning a name allows you and other operators to better recognize
the feature during history editing.
Use caution when renaming and replacing features
CAUTION:If you rename or replace a feature that is parametrically related
to another features by its name, the related feature and all of its children
will not regenerate properly. If you are unsure, perform a History
Regen after renaming the feature or use the History
Manager to view the feature's parent/child relationships before renaming
or replacing it.
What you can do: If a dependent feature references the replaced feature by its name, you can use Rename Feature to rename the new feature to that of the feature it replaced. This should allow the dependent feature to regenerate properly.
Using the heal topology commands
The
commands on the Heal side bar
are ideal for checking and healing imported part geometry such as those
generated from IGES neutral files. Be aware that many of these commands
modify the topology of the part (e.g., moving or deleting vertices, edges,
or tiny faces) within acceptable tolerances.
Commands that save the layer visibility state
The
Inquire Mass Properties, Parting
Lines from Silhouettes, and Parting
Lines from Plane Intersection commands save the active layer visibility
state at the time they are executed and restores this visibility status
when they are regenerated. These commands have an option to pick all components
or all faces with a middle-click of the mouse (i.e., null input). In these
case only components and faces on visible layers are selected.
What you should know about cutting, copying and pasting history operations
Any
given block of operations cut or copied from the history into the 3D clipboard
may contain references to entities that are not included in the block
of operations. Also, the cut/copied operations themselves have unique
id's that may not be valid outside the context of the history from which
they were extracted.
When operations are "cut" from the history, their unique id's and entity references are left unchanged. This gives them the greatest chance of regenerating if they are reinserted into the same history. If they are inserted into another part's history, they will only regenerate if they do not reference entities outside of the "cut" block of operations. If they are reinserted again into the same history, their ids are upgraded to make them unique. This is done to avoid any conflicts with the previously inserted copy of operations.
When operations are "copied" to the 3D clipboard, their unique id's and entity references are modified so that they do not overlap with the original operations that remain in the history. They can be reinserted in the same history, or another history, without conflicting with existing ids. They will not however, regenerate properly if they reference entities outside the block of copied operations.
What you should know about adding shapes with open and closed profiles
Depending
on the state of the active part (solid or surface) and the feature profile
(open or closed), VX will perform either a boolean operation (for solids)
or a sew operation (for surfaces). In VX, a solid feature will be created
when the profile adheres to one of the following conditions:
A closed profile with both endcaps
An open profile with offset and both endcaps
An open profile with boundary faces (endcaps are forced)
A condition to consider when using boundary faces
The
"Boundary Face" option is used to make sure that extrude,
revolve and sweep distances are long enough to intersect the specified
face completely such that subsequent boolean operations make sense. However,
there is a condition that may appear to be in error but is in fact working
correctly.
When the "Boundary Face" option is used to specify the start distance, and then the end distance is further away but ON THE SAME SIDE of the face, then the start distance will move to the other side of the face. This is so because VX attempts to make the feature INTERSECT the specified face, as it was originally specified. This is not an error. After all, if this did not happen, the feature would not intersect the boundary face at all, and the original intent would have been ignored.
Should I accept the partial results when filleting and chamfering?
During
solid fillet, chamfer and thread operations, if the operation fails, the
prompt"Filleting (or
chamfer) failed - partial results?"is displayed. If you select Yes, a partial results of the operation
is created. The partial results consist of the new face fillet or chamfer
sewn together into a separate shell and the topology split and/or extended
as much as is possible. If you select No, an error message is returned.
This allows you to still create as much fillet or chamfer geometry as
possible even if a failure occurs.
It would not hurt to accept the partial results and review them. You may be able to use some of them even if you have to tie them in manually. It will also indicate where the problem areas are. You can then undo the operation, correct the area and try the operation again.
Command-line command to assign new unique labels to faces and edges
Using (Ctrl) and (Shift) keys for selection (History and Layer Manager)
How to add, modify or delete a fillet radius attribute after the fillet is complete
If the form will not close during the Insert Custom Input command
If you don't use a Custom Input operation for a Custom Feature
When
prompted to select history-generated entities (shape, face, edge, curve,
point, sketch, component), you can select a feature operation from the
History Manager. Entities
generated by the operation that satisfy the active Pick Filter setting
will be automatically be added to the current entity input field, replacing
existing entities.
When the input field is regenerated, a new list of entities of the specified type will be
re-extracted from the selected feature. This is another way to associatively link one feature to another in the history. It is a faster way to pick up all the entities created by a feature than using the "Attribute" Pick Filter plus "Pick All." For example, when prompted for edges to fillet, picking a feature from the History Manager would automatically select all edges associated with that feature.
Sketch-driven network of rods.
If
you pick a sketch during entity input in part edit mode, curves belonging
to the sketch will be added to the current input field. An
example of where this might be used is in the creation of rod features.
When prompted
for rod drive curves, selecting a sketch will cause rods to created along
every curve in the sketch. Thus,
a sketch can be used to control the number and placement of a network
of rods (i.e., cooling channels in a mold).
Make sure base lines, arcs, circles and curves are properly constrained
You
should ensure that the base line, arc, circle, or curve that you are constraining
to is also properly constrained. For example, placing a 2D
Anchor Constraint on the base curve will fix it in position while
other geometry is constrained to it. The base curve may also be constrained
to other geometry thus determining its position. A base curve that is
unconstrained may produce unpredictable results when the constraints are
solved.
A quick way to dimensioning to external reference points
While
selecting point input at the sketch level, if you press and hold the F7
key, the point input mode will temporarily change to Critical
and Smart Pick (if On) will snap to external reference
points anywhere in the active part or assembly where geometry is visible.
These are critical points that lie outside the sketch plane.
This procedure will project a reference point onto the sketch
plane similar to the Project a Reference Point
command. It's a quick way of including external reference points in your
dimension scheme. The external reference point created is of course parametrically
driven. If the external geometry is modified and the critical point is
moved, the reference point and sketch dimensions will adapt accordingly.
You can select points on multiple sketches to drive features
Point
entities within sketches are displayed when the sketch is not active.
This allows you to use sketches to lay down reference points on different
datum planes, then use the points to drive 3D part features.
Bill of materials - Using non-graphic components (e.g., paint, grease)
Assembly Parts List - Using non-graphic components (e.g., paint, grease)
All parts referenced by an assembly are listed in the VX Search Path Form
When
a component is merged into the active part, a copy of its geometry is
merged. The component itself is not deleted. It is just blanked. If the
component is changed, the next time you perform a History
Regen, the parent part will re-merge the new component data.
Using leader callout arrows with other dimensions or geometry
Why you should not use the color RED as the dimension color
3D
layout views can be dimensioned with the available drawing sheet dimensioning
tools. When a dimension is created, there is an associativity established
between the dimension and the geometry of the view. If the geometry associated
with a dimension is removed after regenerating the layout view, the dimension
is displayed inRED
to indicate that the associativity has been broken. For this reason, the
colorRED
should not be used as the dimension color.
Sheet scale verses layout view scale
The
drawing sheet scale factor is ignored completely
within a layout view, and the individual layout view's scale sets the
scale factor. The drawing sheet scale factor only applies to geometry
that has been added to the drawing sheet directly, and does not belong
to any layout view.
Use caution when deleting a layout view
CAUTION: Layout views
may contain dependencies to other views or geometry. If you try to delete
a layout view that contains dependencies, you will be warned that doing
so may affect other views or geometry. You should proceed with caution.
