CATIA Spaceframe

[Horace]

Has anyone had any experience with drawing spaceframes or any sort of structures with CATIA?

We're having trouble with assigning custom section profiles to the lines drawn. We did the whole line drawing thing using the wireframe workbench. Then we assign tubes to it using the structural design workbench. However none of the profiles that came with CATIA is anywhere near the tube dimensions that we use for CATIA.

In Solidworks, it's pretty easy with the weldments feature. We're trying to find an equivalent of the weldments feature but in CATIA instead.

[Horace]

Has anyone had any experience with drawing spaceframes or any sort of structures with CATIA?

We're having trouble with assigning custom section profiles to the lines drawn. We did the whole line drawing thing using the wireframe workbench. Then we assign tubes to it using the structural design workbench. However none of the profiles that came with CATIA is anywhere near the tube dimensions that we use for CATIA.

In Solidworks, it's pretty easy with the weldments feature. We're trying to find an equivalent of the weldments feature but in CATIA instead.

[Garre88e]

We do it a little differently..

Once we have the chassis lines drawn we use the Generative Shape Design workbench to give the tubes a round profile. Use the 'sweep' command, click the round profile at the top of the dialog, and change the subtype to 'center and radius.' then we go into part design and apply a thick surface to the profile, the offset being the tube thickness.

I don't have experience doing it the way you did, this is how we've always done it.

Hope that helps

[exFSAE]

<BLOCKQUOTE class="ip-ubbcode-quote"><div class="ip-ubbcode-quote-title">quote:</div><div class="ip-ubbcode-quote-content">Originally posted by Horace:
Has anyone had any experience with drawing spaceframes or any sort of structures with CATIA?

We're having trouble with assigning custom section profiles to the lines drawn. We did the whole line drawing thing using the wireframe workbench. Then we assign tubes to it using the structural design workbench. However none of the profiles that came with CATIA is anywhere near the tube dimensions that we use for CATIA.

In Solidworks, it's pretty easy with the weldments feature. We're trying to find an equivalent of the weldments feature but in CATIA instead. </div></BLOCKQUOTE>

None of the tube profiles in Solidworks are near FSAE dimensions either, or at least they weren't the last time I used it. However, in Solidworks, you can make custom tube profiles by saving them in the right place.

Must be something similar for CATIA?

[Horace]

<BLOCKQUOTE class="ip-ubbcode-quote"><div class="ip-ubbcode-quote-title">quote:</div><div class="ip-ubbcode-quote-content">Originally posted by exFSAE:
<BLOCKQUOTE class="ip-ubbcode-quote"><div class="ip-ubbcode-quote-title">quote:</div><div class="ip-ubbcode-quote-content">Originally posted by Horace:
Has anyone had any experience with drawing spaceframes or any sort of structures with CATIA?

We're having trouble with assigning custom section profiles to the lines drawn. We did the whole line drawing thing using the wireframe workbench. Then we assign tubes to it using the structural design workbench. However none of the profiles that came with CATIA is anywhere near the tube dimensions that we use for CATIA.

In Solidworks, it's pretty easy with the weldments feature. We're trying to find an equivalent of the weldments feature but in CATIA instead. </div></BLOCKQUOTE>

None of the tube profiles in Solidworks are near FSAE dimensions either, or at least they weren't the last time I used it. However, in Solidworks, you can make custom tube profiles by saving them in the right place.

Must be something similar for CATIA? </div></BLOCKQUOTE>

I thought it would be something similar for CATIA as well, unfortunately it isn't so simple. I found the folder where all the resolved sections are located, and tried adding my own, but they did not show up in the program. I also tried editing the catalogs and added my own parametric sections, no luck either. I think I might need to resolve the parametric sketch to all the different sketches and then add the parametric sketch to the catalog, but in the help files it says something about entering the CATIA environment file and I have no clue what it is.

[Hub]

Like Horace I've tried to add my tube profiles in structural design without success.
Horace do you found a solution? or someone else?

It's more simple in solidworks.

[BeaverGuy]

Because of your difficulties playing with the structural sections I was inspired to play with it at work. And I figured out how to add a new family of profiles to the catalog. First I will explain the easy way to adjust the profiles then I will explain the correct way.

The easiest way is to edit the profiles that you allready have. To do this go to Program Files\Dassault Systemes\B18\win_b64\startup\EquipmentAndSystems\S tructure\StructuralCatalogs\AISC\DesignTables for 64bit or Program Files\Dassault Systemes\B18\intel_a\startup\EquipmentAndSystems\S tructure\StructuralCatalogs for 32 bit. If you want to edit the pipe profiles for tubing open AISC_Pipes.txt with a spreadsheet program as tab delimited. You can either add more profiles to the spread sheet or replace exiting profiles. For the pipes profiles the only values that are used for generating the geometry are PartNumber, Tw, and vxm. After editing the spreadsheet save it. Now open the AISC_Sample.catalog file. Double click the profile family that you edited, in this case Pipes. Now go to Insert&gt;Add Part Components... A "Part Family Definition" dialog box comes up click on Select Document navigate to ...\AISC\Models select AISC_Pipes.CATPart and click open. Your profiles have now been updated and you should save the catalog.

To add the profile properly you should create a new part with an asociated sketch. Then link a design table to that part. That part is now your seed part; you should add it to the ...\AISC\Models folder or similar. Don't ask me how to create design tables because I've only done it once and that was quite a while ago. Now open your catalog or create a new catalog go to Insert&gt;Add Part Family... A "Part Family Definition" dialog box comes up click on Select Document navigate to where you saved your seed part, select your seed part and click ok. You should now have a new part family with various configurations.

If you don't want to mess with creating a new design table driven sketch, but you want to preserve the integrity of the original files, you can start with the parts that have allready been created. First Save the design table text file as a copy with a new name. Then open the seed part from ...AISC\Models in Catia and save that as a new part with a different name. Now open the new cat part that you just created and go to Edit&gt;links click Replace navigate to and select the new design table text file and click Open, then click OK. Now save the part.

Hope this helps.

[Hub]

Thanks BeaverGuy for your response http://fsae.com/groupee_common/emoticons/icon_smile.gif

I've tried your easy way but it don't work.
First when I select a a pipe profile in structural design I have 10 choice but 37 in the AISC_pipe.txt table. If I add or edit a profil in AISC_pipe.txt and follow your step it's don't work on structural design and my section remain the same. I've edit D, Tw, vxm. I've tried also ti edit directly the sketch and same as above.

Also do you know witch parameter Tw, and vxm control?

[Hub]

If I edit sketch in folder \Program Files\Dassault Systemes\B19\intel_a\startup\EquipmentAndSystems\S tructure\StructuralCatalogs\ModelsResolved , it's work, but not in \Program Files\Dassault Systemes\B19\intel_a\startup\EquipmentAndSystems\S tructure\StructuralCatalogs\AISC\ModelsResolved

But I need to kept the original file name and it's not practical. A method to change or add profile name BeaverGuy?

[Hub]

The structural design profils are located in: \Program Files\Dassault Systemes\B19\intel_a\startup\EquipmentAndSystems\S tructure\StructuralCatalogs\Materials\StructureMat erialSpecifications.catalog

And I can create a new family but if I create a profile it don't appear in structural design. if a modify an existing profiles the profiles is selectable but dimensions stay as before the edit. Perhaps I need to modify a pipe profiles file but where?

[BeaverGuy]

Sorry that didn't work, I don't have access to the Structural Design Workbench only the catalogs and sections. When I browsed into the AISC catalog and inserted a new part from the catalog the directions I gave worked. The instructions I gave updates the AISC catalogs but it appears that there is no link between that catalog and structural design profiles catalog. So what you need to do is find the resolved structural design profiles catalog and add your resolved sections to that catalog. There is a batch file to generate resolved sections from parametric sections but it doesn't work on 64bit machines unless you make a copy of the C:\Program Files\Dassault Systemes\B18\win_b64\code\bin and put it in a new directory C:\Program Files\Dassault Systemes\B18\intel_a\code\bin. This is the Catia help that Horace was talking about. To find the name of the Environment right click on the shortcut you use to open Catia, on the shortcut tab under target you will find a string containing "-env CATIA.V5R18.B18" the section that follows -env is the name of the Catia envirornment file.

To generate the resolved sections using the batch file open a windows command prompt.

Type cd\ c:\Program Files\Dassault Systemes\B18\win_b64\code\command press enter, if 32 bit use intel_a instead of win_b64.

Now type CATCloGenerateResolvedParts.bat -env CATIA.V5R18.B18 "c:\directory of parametric part" "c:\directory of resolved parts" -appl Structure press enter. The batch file will now start and another window should pop up and it will start creating resolved parts. When that is finished you need to add those parts to the structural shapes catalog.

You could probably manualy add resolved shapes but, as per the catia help in order to be available when added to the catalog they must conform to the followng :"Structure parts must have a parameter called "ProfileType". New or existing parameters "PartNumber" and "SectionName" will be valuated with the part number from the design table. New parameters called "FamilyName" and "CatalogName" will be created unless they exist already (the name of the parametric part will be used to valuate these parameters if they do not exist, using the following naming convention: catalogname_familyname.CATPart). The "FamilyName" parameter is used by the automatic catalog creation function (Create/Modify Catalog) to place parts under different catalog families."

[Hub]

I can't use the bat file, and the procedure is quit complex. I will edit sketch from StructuralCatalogs\ModelsResolved. It's note a proper way to do but it's work and it's more simple.

Thank you Josh for taking time to help me with these problems.