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HIDING DATUMS in Catia 4

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designmr

Mechanical
Nov 29, 2005
230
Anyone know how to HIDE completely the DATUMS and keeps them hiding?

I was sent a file (.product) with hundreds of parts, I want to just hide ALL the DATUM PANELS at once.

The version I am using is CATIA, Version 5, rev 9. Seems you can hide the datums, and save the file. Once you call it up again, the datum are BACK again, same with contraints.

Thanks
 
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From the Menu, choose Edit -> SEARCH . In Workbench select Part Design, then in TYPE select Plane and hit the binocular. Select them and Hide.

You must save all the parts of your assy if you don't want them ON next time you'll load the assembly.

-Hora
 
Hora, will this HIDE all the parts at once, or do I need to go one by one?

Thanks
 
If you don't like working in menus, (like I don't) you can also use the power input.

In the little white box at the bottom of the screen, type "t:plane". (no quotations marks) When they all select, right click any one plane in the tree, and select "hide/show".

Same effect, different (faster) method.

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Catia Design|Catia Design News|Catia V5 blog
 
Good tip Solid7, but unfortunately this does not work in Assembly Design. Works great in Part mode (at least in V5 Release 15)


-Hora
 
Yes, good point. (I forgot all about it not working in assembly)

You can make a script (very easily) to hide/show planes in an assembly, based on the search you did, or check this out:


I have a similar script set up as a toolbar icon.

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Catia Design|Catia Design News|Catia V5 blog
 
Does anyone know why this doesn't work in assy mode but ok with power input in part design?
Is this a setting within the options or a Catia Release issue,
In product environment I have to use the search facility or use VB script.
 
:) Solid7, a star on your shoulder (for your power input).

-Hora
 
because it is searching the currently active document which is a product that does not contain any planes. Try this
t:plane,all
or
t:plane,from
or
t:plane,scr

the bit after the , defines the search scope All being eveywhere, from being selected branch down and scr being only stuff visible on the screen.

 
kboy, I use the following:

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.

It was from Azrael, on another forum, it works great. I'm using an OLD version of Catia V5, rev9...
 
In power input, the coomand t:plane,all does not work for an assembly, but

t:pl*,all

will do the job.

-Hora
 
Ok, I got how to hide them all.....What about to "SHOW", them all again????
 
Same thing... Just do it again.

Or, change the script at this line:

selection1.Search "CATPrtSearch.Plane.Visibility=Visible,all"

TO

selection1.Search "CATPrtSearch.Plane.Visibility=Invisible,all"

AND

VisPropSet1.SetShow catVisPropertyNoShowAttr

TO

VisPropSet1.SetShow catVisPropertyShowAttr

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Catia Design|Catia Design News|Catia V5 blog
 
Thanks solid, I pretty new to Catia, this company does not offer training, everyone is learning on their own.

This is a great site for getting answers I tell you.
 
Solid - yet another company that does not offer training. When will they learn about the ROI of training.

 
This company figured if you already knew Solidworks, you can learn Catia on your own....oh well.

What makes it worse, we have NO access to help files
 
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