This tip is on Add-ins.In the support I have done, I have been amazed at how many do not use or
even know of the add-ins in SolidWorks.Many
are free and just added in when installing a service pack and some are purchased
(i.e. CosmosWorks, CamWorks, PhotoWorks).Since
the latter part of SolidWorks 99 SolidWorks has been adding more and more FREE
add-ins into this list found under Tools à
Add-ins…A list of all that has
been released up to SP6 and a short explanation from SolidWorks help.If you would like more info on any of them please check out the
SolidWorks help under the help pull down in the program
The Add-In module SldTrans 1.0
imports a part or assembly file from Pro/ENGINEER® into a SolidWorks part or
assembly document. The attributes, features, sketches, and dimensions of the
Pro/ENGINEER® part are imported. If all of the features in the file are not
supported, you can choose to import the file as either a solid body or a surface
model.
When importing an assembly, you can
control how to import individual components. Sub-assemblies are supported as
well.
Some known limitations are as
follows:
Only
versions 17 through 20 of Pro/ENGINEER are supported.
The Add-In module SldUg 1.0 imports
the Parasolid information of a Unigraphics® II part or assembly into a
SolidWorks part or assembly document. Only the Parasolid information is
extracted, not the proprietary feature information of a Unigraphics II part.
You can import:
Parts
from Unigraphics II version 10 through version 16
Assemblies
from version 10 through version 15
You have the option to import
Unigraphics files as either one single SolidWorks part, or as multiple
SolidWorks parts.
Single SolidWorks part
One
SolidWorks part is created that has one surface body for each body in the
Unigraphics file.
Multiple SolidWorks parts
One
SolidWorks part is created for each solid in the Unigraphics file
All
tool bodies are placed in a separate part, and suppressed so they don’t
appear in the assembly
One
SolidWorks assembly is created
Parts
located on an invisible layer in the Unigraphics file are suppressed in the
SolidWorks assembly.
The Add-In module SolidWorks 2D
Emulator adds a command line at the bottom of the screen to emulate the AutoDesk®
AutoCAD command line.It has a lot
of the default commands that AutoCAD® has.
Known limitation:
Will
cancel out some of the 3D features in SolidWorks while the add-in is loaded.
(i.e. if a tool button or pull down doesn’t work turn off the add-in an
all should be good.)
This add-in module enables you to
export SolidWorks documents to CATIA® graphics (CGR) files that users can view
in CATIA, CATweb, and DMU Navigator. You can export only parts and assemblies
with the CGR translator.
Support includes CATIA version 5,
release 3, and above.
This add-in module extracts ACIS
information from a DXF part file, if that information exists in the file, and
imports it into a SolidWorks part. SolidWorks does not create the ACIS
information.
Support includes, but is not limited
to, AutoCAD® R14 and above.
Note the following add-in
limitations:
It
is not a 2D to 3D converter.
It
does not import 2D or wireframe data from DXF files.
This add-in module enables you to
export SolidWorks documents to Highly Compressed Graphics (HCG) files. HCG
files, used by CATIA® in CATweb, are optimized for transmission over the Web.
You can export only parts and assemblies with the HCG translator.
The exported files contain graphical
information only; you cannot edit these files.
Support includes CATIA version 5,
release 3, and above.
This add-in module imports AutoDesk
Inventor® part files into SolidWorks part documents. The imported part files
contain only geometry; features are not imported.
Support includes through version
AutoDesk Inventor R2.
This add-in module imports part and
assembly information from a Mechanical Desktop® (MDT) file into a SolidWorks
part or assembly document. You must have MDT installed on your desktop, but it
does not have to be running, to use the MDT translator.
MDT files can contain a combination
of part, assembly, and drawing files. The MDT translator provides different
conversion options, depending upon the contents of the MDT file.
Only MDT version 4 is supported.
NOTE:Because MDT version 4 does not support Windows 2000; the MDT translator
is not supported on the Windows 2000 platform.
This add-in module exports SolidWorks
part or assembly documents to Metastream (.mts) files. You can view Metastream
files over the Internet using the Metastream viewer. The Metastream files
contain the compressed geometry of the model.
The Metastream (MTS) translator also
creates an .mtx file, which is in XML. This is the animation and attribute file
of the model. The exported files contain
graphical information only; you cannot edit these files.
This add-in module imports the
Parasolid information of a Solid Edge® part into a SolidWorks part. Only the
Parasolid information is extracted, not the proprietary feature information of a
Solid Edge part. You can import Parasolid information from Solid Edge parts up
to and including Solid Edge version 8.
This add-in module exports SolidWorks
part or assembly documents to RealityWave's ZGL file format. After exporting the
document, you must save the ZGL file into a RealityWave database (VizStream
Server). This converts the ZGL file into RealityWave’s streaming format that
you then can view over the Internet with the RealityWave viewer.
The exported files contain graphical
information only; you cannot edit these files.
Building parts in the
context of the assembly, using in context references to drive features on your
parts, is very cool... Unfortunately, the two things are mutually exclusive.For instance, if you build a part for a door in the context
of an assembly, you can choose to make the door so the frame it sits in drives
the door's size and shape.However,
if you then use assembly motion to open the door, the geometry of the door part
will change! The door will try to access the driving geometry (the frame) from
the vantage point of its new position, altering the shape of everything. The
work around for this is to leave the door in its original position, RMB click
it, and choose to 'hide' it. Then you CTRL drag another instance of the door
component from the assembly manager into the assembly window, mating the copy in
place (concentric to the hinge, with it's bottom some distance from the
threshold of the door). Now this second instance can be
moved all over without altering the in-context relationships of the door part!In SolidWorks 2000, you can freeze in-context relationships as another
work around for this problem, but if you update the geometry of the doorframe,
the door part will not change. Using two instances of the door component in the
assembly allows you to have your cake and eat it to.
Did
you know you could rotate a view within the drawing?For example if you make a section and want it rotated 90 degrees.Just select the rotate tool.The
same tool as you use to rotate the model in the assembly or part.Choose the view you would like to rotate, click and drag.The view will rotate at incremental snaps with feedback on the screen on
how many degrees you have rotated.Works
great for sections, or to fit on screen or for clarity.
Since I have been so busy
the last few weeks I have missed the last tip time so this tip you get two.Thank you to all that have submitted tips and thank you all for signing
up.Pass the word.
This
week’s first tip comes to us from Dave Murray at CADimensions Inc in NY, USA
Hiding
and showing sketch geometry is independently controlled between a part and its
associated drawing. What this means is if you show a sketch in a part, it will
not automatically be shown in the drawing. Furthermore, sketch visibility can
also be controlled independent of views in a drawing. If you right click on a
sketch in the Drawing Feature Manager, you can show it in that specific view
only, giving you a sketch, which may aid in adding reference dimensions. This is
extremely beneficial when dimensioning ellipses or spline points.
This
week’s second tip comes to us from Stan Heeres at DB Union Pumps in MI, USA
When
creating Assembly Features, the default Feature Scope includes EVERY Component
in the assembly. This greatly increases the rebuild time because every part must
be evaluated during EACH rebuild. This becomes especially important the more
Features that are in the Assembly.
To
avoid this, after building the first Assembly Feature, right click on the
feature, click on Feature Scope and remove all components except those affected.
Make sure to do this after the first Assembly Feature or you will have to
individually delete each component from the list for EACH Assembly Feature.
After doing this on the first feature, all following features will have ONLY
those Components in the list that were in the previous Assembly Feature list.
Simply edit the Feature Scope each time an Assembly Feature is created. This has
cut the rebuild time on the assembly we are working on by 50%!
Do
you have multiple dimensions to change from a 3 place decimal, to a 2 place
decimal at one time?You don’t need to do them separately.“Ctrl select” all or some of the dims you need to change from 3
places to 2 places.Right click on
the last one selected and choose properties.You do not have to uncheck the “use documents precision” box
and then click the Precision… button and change the value and tolerance to 2
places.With multiple dims selected
all that is need to do is, select the dims needed to be changed, right click
properties and uncheck the “use document precision” and click OK.When this is done with more than one dim selected to change the dims
default to 2 places even though you have not changed a number in the Precision
dialog box.
Control + Q (Verification on Rebuild) or
Force Regeneration
Verification on rebuild also
known as Control + Q is a very powerful way to find errors.
This option can be turned on at all times in the options dialog box.Click Tools àOptions à Performance, and select the Verification on rebuild
checkbox.I do not suggest checking
this box because it can slow down all of your work.Because anytime you click the rebuild button it will rebuild
with verification.
Let me explain.A normal rebuild (the little green light on the tool bar) starts from the
last feature worked on in the feature manager tree and rebuilds from there down.A Control + Q starts at the top of the feature manager tree
regardless of what was worked on last and verifies for errors.
If your model looks incorrect (missing lines, not updated, loft or sweep
not looking correct) run a Control + Q.You
can do a Control + Q at any time.A
word to the wise:It takes about 3
time longer for a Control + Q to run than a regular rebuild.A good idea to run before release but not to get into a habit as I have
every time you want to rebuild, unless you only work on small parts and
assemblies.
Just in case I wasn’t clear Control + Q is the Ctrl and the Q button
pressed at the same time.
Creating
models from those old AutoCAD drawings or DXF files.
Open
the drawing that contains the curve entities you want to insert.
Open the part where you
want to insert the entities. (New part or existing part)
Open a sketch and click
Insert à
Sketch from Drawing.
From the Window menu,
select the drawing to make it the active window.
Box-select the entities
with the left mouse button.
Return
to the part window. The entities have been inserted into the active sketch in
the part, and you can now edit the sketch, and use it to make features.
The
drawing uses the same X, Y, and Z points as the original AutoCAD drawing or
translated program for both the drawing part of SolidWorks and the part area of
SolidWorks.
After
the sketch is in the part document, click on the pull down, Tools à
Relations àConstrain all this will add relations of horizontal, vertical, tangent,
and any obvious relations that are needed.This saves you time doing it yourself.!
To
move the sketch to the correct space on the model, you can dimension it and move
it, or use the *modify sketch tool (Tools à
Sketch Tools à
Modify) to place a point to a known X, Y value in the model.
*Modify
Sketch: Allows you to move, rotate, or scale a sketch.
This week’s tip is on the subject of lofting and
sweeping.Instead of a coincident
relationship between your geometry and path, place a pierce relationship between
the point and the path that you are sweeping or lofting on.A coincident relationship can cause problems in future changes or not
allow it sweep or loft at all.
Pierce Relationship: A sketch point and an axis, edge, line, or Spline.
A sketch point and an axis, edge, line, or Spline.The sketch point is coincident to where the axis, edge, or reference
curve pierces the sketch plane.