selecting planes in assembly

[alkemixt]

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

 

[Azrael]

Search for all planes (edit->search in the name field set *plane*), hit the select button and click hide.

A quicker way is to write in the power input: tl* and then set them to hide

 

[jackk]

Alkemixt,

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.

 

[JuhaEdag]

I would do edit-Search (ctrl-F) advanced 1.Workbench GSD
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.

 

[Azrael]

I have a VB script that will set all visible planes in hide, post me your email and try it.

 

[solid7]

I have a VB script that will set all visible planes in hide, post me your email and try it.

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!

 

[Azrael]

Solid7 - Tried to post it on the CATBlog, couldn't find how, probably my fault

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

 

[solid7]

Solid7 - Tried to post it on the CATBlog, couldn't find how, probably my fault

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!

 

[alkemixt]

thans for helping out a newbie..

 

[Azrael]

What do you mean, does the macro dissapear or loose connection to the short cut??

 

[alkemixt]

Hi guys,

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,

 

[alkemixt]

I'm back..
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,

 

[JuhaEdag]

If the part is in cache mode wireframe elements won't show.
Right click the top product and activate design mode and then run macro, Ctrl-f etc.

 

[yusf]

Hi can anyone tell me how i can hide the axis of each part's axis system represented in DMU.. CGR format..in which i have hundreds of axis system..
there can be a macro or some other simple method ..can you help me at this point..

all answers are appreciated..
thx in advance

 

[ferdo]

Hi,

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

 

[designmr]

Azrael, does this work on Catia V5 rev9? Sorry, I know this is an OLD version, but that is what this company has....and they will not update..

thanks

 

[designmr]

Azrael, does your SCRIPT work on V5, rev9???

I know its an old one, but this company will NOT update

 

[solid7]

The scripts posted can be easily obtained by recording a macro using the "search" function.

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.

-----------------------------------------------------------
Catia Design|Catia Design News|Catia V5 blog

 

[catiajim]

Also note: If your employer is telling you to use an illegal version of CATIA, FIND A NEW JOB. It's not worth working for a company that is not willing to utilize legal versions of software. There are plenty of legitimate companies out there that are using CATIA and have enough ethics to pay for their software. Any company willing to steal from a software vendor is also probably not above stealing from its employees.