selecting planes in assembly
selecting planes in assembly
(OP)
Hi,
i have a catprod that has over 200 cadparts, and all of them have x,y,z planes showing.
Is there a quick way to hide all the planes.
The selection filter doesn't have planes, and hiding one at a time will take forever. Why isn't there a hide/show point, line, planes, etc in the assembly like there is in part desing?
thanks
i have a catprod that has over 200 cadparts, and all of them have x,y,z planes showing.
Is there a quick way to hide all the planes.
The selection filter doesn't have planes, and hiding one at a time will take forever. Why isn't there a hide/show point, line, planes, etc in the assembly like there is in part desing?
thanks





RE: selecting planes in assembly
A quicker way is to write in the power input: t:pl* and then set them to hide
RE: selecting planes in assembly
I agree with Azrael's suggestion (but I type: t=pl*), but be prepared to wait while it goes through all the parts in your assembly.
I suggest you start a company-wide practice of hiding all planes (and other construction geometry) before saving a part.
RE: selecting planes in assembly
2. Type Plane 3. Attribute Visible 4. Search 5. Select 6. Hide/Show.
The attribute visible is necessary because it would oherwise also select planes already in Hide.
RE: selecting planes in assembly
RE: selecting planes in assembly
Even better idea - post it on the CATBlog, and share it with everyone. (asking kindly)
I'd love to see more people post - especially VB and CATscripts.
**************
Check out CATBlog!
RE: selecting planes in assembly
Alkemixt - Try this:
Go to Tools->Macro and choose create, set to VB script and name your macro. Paste this:
-------------------------------------------
Language="VBSCRIPT"
Sub CATMain()
Set productDocument1 = CATIA.ActiveDocument
Set selection1 = productDocument1.Selection
selection1.Search "CATPrtSearch.Plane.Visibility=Visible,all"
Set VisPropSet1 = Selection1.VisProperties
VisPropSet1.SetShow catVisPropertyNoShowAttr
End Sub
--------------------------------------------
Now you can run it and test it
If you want to add it as button, go to custimize and under the commands bar there should be a category named macros (left field), in the right field pick your macro and hit show properties, change icon name if wanted and pick and icon in the list. Now just just drag the macro from the commands field into an existing toolbar in Catia. Of course you can also make your own toolbar
RE: selecting planes in assembly
My activity log is showing that you successfully registered. All that you need to do now, is follow the 'admin' link, and from there, you should have no trouble finding the 'add item' field.
Thanks for your input.
**************
Check out CATBlog!
RE: selecting planes in assembly
RE: selecting planes in assembly
RE: selecting planes in assembly
All your suggestions work to certain extent but it does not select all the planes, only a handful out of over 1500 planes. Is there a limit as to how many can be selected or seached?
And i noticed that if I select the top product, it only find a few, and when i hide them and perform search again, it doesn't find any.
i wish i could show how many planes there are in my product..it's almost insane, and it interferes with the section views.
thanks,
RE: selecting planes in assembly
it seems like if I double click on the part, and run the macro, it finds a handful of new planes and hide.
Is there a way to search through all the parts under the main product tree?
or should i load everything then run the macro perhaps?
how do i load everything? :)
thanks,
RE: selecting planes in assembly
Right click the top product and activate design mode and then run macro, Ctrl-f etc.
RE: selecting planes in assembly
there can be a macro or some other simple method ..can you help me at this point..
all answers are appreciated..
thx in advance
RE: selecting planes in assembly
I've made a modification in the CATScript writen by Azrael sa now its hiding also axis systems and open body features.
'------------------------
Language="VBSCRIPT"
Sub CATMain()
Set productDocument1 = CATIA.ActiveDocument
'*******************hide Plane
Set selection1 = productDocument1.Selection
selection1.Search "CATPrtSearch.Plane.Visibility=Visible,all"
Set VisPropSet1 = Selection1.VisProperties
VisPropSet1.SetShow catVisPropertyNoShowAttr
'*******************hide AxisSystem
Set selection2 = productDocument1.Selection
selection2.Search "CATPrtSearch.AxisSystem.Visibility=Visible,all"
Set VisPropSet1 = Selection2.VisProperties
VisPropSet1.SetShow catVisPropertyNoShowAttr
'*******************hide OpenBodyFeature
Set selection3 = productDocument1.Selection
selection3.Search "CATPrtSearch.OpenBodyFeature.Visibility=Visible,all"
Set VisPropSet1 = Selection3.VisProperties
VisPropSet1.SetShow catVisPropertyNoShowAttr
End Sub
'-----------------------------------
Regards
Fernando
RE: selecting planes in assembly
thanks
RE: selecting planes in assembly
I know its an old one, but this company will NOT update
RE: selecting planes in assembly
If your employer doesn't want to "upgrade", that's what you'll have to do. R9, aside from being one of the most readily available cracked (and heavily downloaded) versions of Catia, is also long past its support date. Not suprisingly, most - if not all of us, no longer have it.
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RE: selecting planes in assembly