Unsupress All Parts/Subassemblies (Macro Maybe) 2

[BodyBagger]

Hello all,
I did a search on this and it appears that it has not been touched on since 07 so I would like to revisit it. We get some large assembly models from vendors and they tend to have many levels of subassemblies, etc. These assemblies tend to have a lot of suppressed parts and I would like to do an "Unsupress All Parts & Assemblies" for a specific configuration. Is there a way of doing this in SW2010 rather than drilling down and doing them one at a time? I found a Lenny macro but it was written for SW03 and it locks up 2010 tighter than a drum.

Thanks in advance,
BB

 

[Gupta65]

Not sure of macro, but try saving your assembly as iges or parasolid. In that case you'll be promoted with a message for unsupressing the parts, just click OK and unsuppress the parts.

Also if you know, you can edit the macro to suit the needs

Deepak Gupta
SW2009 SP4.1
SW2007 SP5.0
MathCAD 14.0

 

[MFDO]

Tools/Component Selection/...

RBM the selected and unsupress.

Michael Fernando CSWP
Tool and Die Designer
SWX 2009 SP3.0 X64
PDMWorks 2009
Logopress3
FastForm Advance
FormatWorks

 

[jobiewan99]

MFDO,

That is friggin fantastic..... Thanks for sharing! It even finds parts that are suppressed in subassemblies and parts in folders.

Wish I would have known about that command earlier!

Solidworks 2009 SP5.1
4GB Ram
Quadro FX3700
2.66GHz Core 2 Quad XP Pro SP2.0

 

[mjcole]

If you use Customize Screen
Quick way to open that is hit s or your shortcut bar key and right click the bar and select Customize...
Then when the Customize Screen window is up
drag the

Commands - Sketch
Select tool icon shown at Top Left of Buttons grouping to your main Toolbar or Shortcut Bar, there is a Select Suppressed option which can be selected from the flyout

Use that with Right Click
Unsuppress icon#3, Component Properties icon#6
+s SSet to Resolved in Feature manager

+e Set to Resolved in Display

Component Properties
[Suppression State
select (*)Resolved radio button
OK

The Advanced Select... tool allows you to create rules for parts you want to select based on File Status, Component Status/Display, Configuration Names etc.

If you haven't work with advanced select you may be able to set up rules that can be used in any of your assemblies or Exported and Imported from the Query.xml files that SolidWorks saves the Define Search Criteria

You can import the attached xml file by going to
Select > Advanced Select...
Manage Searches
[Import Searches] Browse to and open the XML file I attached to this post

To see what info is used for the search you can select the Define Search Criteria and pick name of the Saved Searches from the Name of Search: Drop Down

Manage Searches gives the option to check off favorites any checked items will appear under the Menu Button for Advanced Select...

Michael

 

[gp13]

If you do want a one-click macro for this, it's pretty simple. I was recently building a macro where my first step does what you ask. Here is that section, if you want it. I'm using '09 by the way.

Dim swApp As ISldWorks
Dim MyAssy As SldWorks.AssemblyDoc
Dim MyComps As Variant
Dim i As Long

Sub main()

Set swApp = Application.SldWorks
Set MyAssy = swApp.ActiveDoc
MyComps = MyAssy.GetComponents(True)
For i = 0 To UBound(MyComps)
retval = MyComps(i).SetSuppression2(swComponentFullyResolved)
Next i

End Sub

 

[BodyBagger]

Thanks to all for the input and suggestions. So far the macro from gopack13 worked the best for my needs. Keep the suggestions coming if there are more.

Thanks again,
BB