Assembly hole problem 1

[abeschneider]

For some reason, when I try to create an assembly hole feature, I cannot select faces, only edges. (I searched the forums and saw a couple people had mentioned this problem, but I saw no positive solution).

Has anyone had an issue like this with assembly hole command? How can I get this working?

Thanks.

 

[DBezaire]

Unsure Abe , I have not seen this. Are in the active assembly where the parts exist in the tree?

Regards,
Derek

 

[abeschneider]

Derek,
Sorry, I don't understand your question. Can you restate it?
Thanks.

 

[DBezaire]

Abeschneider - The assembly design workbench is looking for a publicated item. Publish out the face where you want the hole to start.

Regards,
Derek

 

[abeschneider]

Derek -
That works! Man, I should have thought of that (I have Catia set up so that I can only link to published elements, so this should have been 1st on my mind)...

Problem though - This only seems to work on flat surfaces; it won't allow me to place a hole on a published cylindrical face. (Perhaps this is because you can't create planes in assembly "product" mode?)

I guess a workaround to this new problem could be to create a datum plane perpendicular to the cylindrical face in the part with cylindrical face, then publish the plane out, then do the assembly hole relative to this plane... I will try this out.

 

[solid7]

The assembly design workbench is looking for a publicated item. Publish out the face where you want the hole to start.

Is that true? I'm popping assembly holes left and right, and I've never published (or publicated) anything. It works just fine for me on a selected face.

Is Abe's situation different than mine?

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CAD design engineering services - Catia V4, Catia V5, and CAD Translation. Catia V5 resources - CATBlog.

 

[DBezaire]

Solid7 - Tools-Options-Infrastructure-Part Infra - Restrict external selection with link to published items.
This also applies for Assembly Symmetry

Abe - if you turn off this option you should be able to pick the cylinder face.


Regards,
Derek

 

[DBezaire]

Abe - disregard the last post. Even with the option off you will not be able to use the round face of a cylinder. Sorry

Regards,
Derek

 

[abeschneider]

OK, so publishing a plane perpendicular to the axis of the hole going through the cylindrical face works, but I can't seem to figure out how to reposition the hole...It just snaps to the center of the plane and the option for the Positioning Sketch in the Assembly Hole dialog box is greyed-out.

Help?

 

[abeschneider]

OK, I am answering my question in the last post, about how to position assembly holes.

When you create an assembly hole, the operation creates an entity in the first "affected part" called "Positioning Sketch - xxxx" (ie: "Positioning Sketch - Assembly Hole.1").

This Positioning Sketch is automatically added as an External Reference to all the other "affected parts" in the Assembly Hole operation.

So, to reposition an assembly hole, go to the Positioning Sketch in that 1st part.

Sheesh, the CATIA help files could have been a LITTLE more thorough in describing this functionality...

 

[solid7]

Abe - disregard the last post. Even with the option off you will not be able to use the round face of a cylinder. Sorry

I got it to work just fine. You have to have more than one part in the assembly tree, but it DOES work...


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CAD design engineering services - Catia V4, Catia V5, and CAD Translation. Catia V5 resources - CATBlog.

 

[abeschneider]

Solid7, are you able to place assembly holes on a cylindrical face WITH the option to only link to Published elements toggled on?

 

[solid7]

Nope. I don't use published elements.

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CAD design engineering services - Catia V4, Catia V5, and CAD Translation. Catia V5 resources - CATBlog.

 

[DBezaire]

Sorry I wasn't clear - option off and you can put a hole through a cylinder - option on - even if you publish the face- still no hole.

Derek

 

[abeschneider]

Right, I'm getting the same behavior as you Derek when using publish. Easy work around is to create the normal plane in the part, then publish the plane and use it to place the hole.