Project partbody

[jmuriarte]

Hello:

Can I project a partbody in a plane? I can intersect a partbody with a plane, but I need to project it.

Thanks

 

[DBezaire]

Jmuriarte - In GSD use the extract function - no propagation for the element type perform a search (CNTRL F)
Search options - Workbench:Topology Type:Edge Look:In Part
Search and Select
This gives you boundary extractions of the entire solid.
Project these items to your plane.

Regards,
Derek

 

[jmuriarte]

Thank you very much Derek. But I need the boundary to be updated when I modify de geometry of the part body.
I am trying to create a volume arround the partbody as a rough. To include it in the BOM.I know there is a command in machining but we dont have the license.

 

[solid7]

Don't know what your part looks like - but this is one of the functions of the "reflect line" command. Well, at least to be able to extract what boundaries look like from a particular viewing plane. If you can extract reflect lines, you can project them to a plane.

The other option is to project the partbody into a sketch plane. Once again, you have not mentioned what your part looks like, but this is a common solution. (at least for me)

You will run into problems with both methods if the boundary faces are perfectly square; although that makes projecting face by face a piece of cake.

Using any of the above methods, without toggling the "datum elements" button, should give you waht you are after.

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[jmuriarte]

Ok:

I will try to explain you better. I want to create a volume arround a partbody made with catia operations(Pads, splits...). When I design parts in an assy of a tooling I must write in a paper the limit dimensions of each part(The volume arround the part). This volume should update as I change the partbody geometry.

 

[solid7]

I don't have any trouble understanding what you're doing. What part of my explanation didn't you understand?

Once you get the outer limits of the part, you can "nest" the shape in a block, or whatever your stock shape is, in a sketch plane, after projection.

What shape do you want? A square? A constant offset? What is the shape of the space between the outer limits of your part, and the outer limits of your material? (the cross section that defines the volume)

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[jackk]

Jmuraite...

I've got two possible solutions for you:

1. There is a command called "Rough Stock" that computes the minimum stock size based on your partbody, and it creates a volume of faces for your reference. I recall it requires a NC license, but I forget which one. You can find some more information about it by doing a search in the help files.

2. When you do an Inertia analysis, CATIA draws a 3D box around the part. If you keep the measures, you will find 3 BBL values at the very bottom of the tree. These are the Boundary Box Lengths in the x, y and z directions. (I think this is what you're looking for?) You may have to play around with an axis to change the orientation.

I don't recall if either of these solutions provide the update capability you want. I'll let you check them out and report back. But both are very quick and easy to use.

 

[solid7]

jackk - nice suggestion, but there is no option to create the geometry from the inertia analysis, and even if there were, it is not associative.

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

 

[DBezaire]

solid7 - in my journeys I have come across a script that creates an associative bounding box to a solid or joined surface. It adds 1mm wall stock and uses an axis system for orientation. Can you post this?

Regards,
Derek

 

[solid7]

Sure - I would be happy to.

http://2htts.com/CATBlog

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

 

[jmuriarte]

Thank you very much Solid7 and DBezaire.

I am not very use to work with catscripts. How must I use it?

 

[solid7]

Save it someplace - suggest using a folder called "CATSCripts" somewhere on your hard disk. Next, open up the macros dialog, by pressing Alt+F8. When the dialog opens, there is a button called "macro libraries". Press it, and select "add existing library". Browse to your folder, and press OK.

TO run it, you simply need to find it in the list of macros, (which will now be available, since you added the folder as a library) and select "run".

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

 

[jmuriarte]

Great Macro solid7 thank you very much. It is very usefull for us. We are trying to parametrize a very special kind of toolings for sheet metal.

I have another question about your macro.Could be posible to modify the part with new operations like pockets, pads.. and update the bounding box?

 

[solid7]

jmuriarte:

The resultant geometry of this macro cannot stay associative to later changes. (it's not logical)

By the way - you owe Derek the thanks for that one. And whatever Frenchman that wrote it.

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

 

[jmuriarte]

And if you run the macro using published partbody or face?

 

[solid7]

I have no idea; I'm not familiar with Published elements, since I work mostly in the world of one-off design.

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

 

[solid7]

Derek - I am not getting this macro to work properly. If I understand correctly, it's supposed to add 1mm of excess all the way around the part envelope, correct? When I run it, not matter where the axis is, or which face I select, it always makes the box "net" to the part periphery. The box is created with sweep, and it is then converted to a close surface, via an implicit planar face closing on both ends of the box.

Anybody else having this issue? Am I misunderstanding something?

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

 

[DBezaire]

Solid7, I might have sent a modified copy. Internally we issue net sizes.