Tubing or Piping for V5/R5

[rgf1310]

Does anyone know best way of doing tubing and/or piping design with bends
using V5/R5. I got as far as pasting a “Sketcher workbench file” .CATPart
consisting of two lines “L” shape with a radius connecting the two line gather
into a “Structures workbench” and using “Member on Support”. I can only do solid
segments related to each wireframe. In the V4 we use to concatenate the wireframe to project a FAC.

 

[13910634301]

Hi:
Can you access to V5 Generative Shape Design? My suggestion is using the sweep function under it.
First creat the 3D routing curve and then click the sweep icon choose the circle type , select center curve and enter radius ,you will get the surface of the pipe . If you wanna get the solid , u should select the workbench of Part Design , close the surface and shell it or add the thickness to the surface .

 

[rgf1310]

Excellent advise! Now to work on my wireframe skills.
Question. On the later releases, V5/R8 does tubing and/or
piping apply K-factors for material growth under bending
condition?

 

[13910634301]

As I know, we can only find K-facors definition in the CATIA V5 Sheet Metal Design and most of them are plate sheet metal. What I have is V5R9, so you can't bend your piping with the K-factor I think.

 

[13910634301]

If you have some Microsoft VBScript experience,maybe you can get what you want with catscript. Find two files called PslTubingExtract.CATScript and PslTubingExtractTemplate.xls in your CATIA installation folder. And copy them in a tem folder. Click Tools - Macro - Macros. Select PslTubingExtract.CATScript and click Open. This will again display the Macro dialog box. Select PslTubingExtract.CATScript and click Run. Data will be extracted from the bendable objects and displayed in an Excel worksheet, part of which is displayed below. (The application will create the table, but you must have Excel installed!) If you have some Microsoft VBScript experience,maybe you can change the CATScript and add the K-factors.

 

[BKelly5300]

Presumably the best way to create tubing would be to use the Tubing Design workbench, wouldn't it? It does not require you to build a centerline then sweep around it, it's more like the V4 Tubing function. As far as having K-factors, springback factors, extracting tube data and other such topics - good question, I'm trying to figure that out too, and there is not much documentation , or help available, on the subject of tubing in V5.
Sorry not much help but there is an entire workbench just for creating tubing. As near as I can tell it doesn't work too well yet.
Good Luck-
Kelly

 

[rgf1310]

Thank you 13910634301, on the Microsoft VBScript I have no experience with that. I think the best thing would be to up grade to R9 and run with that. Thanks for the Info..

BKelly as far as I know, V5R5 has a Structures Work Bench that uses grids and splines to sweep a solid shape. Again soon as I can up grade to R7-R9 I'll be looking into that K-Factor as well

Cheers everyone!

 

[BKelly5300]

rgf1310-
Yes, I started with V5R7 so we've always had the Piping Design and other Systems Design workbenches, I noticed right after I posted that you said you have R5, so I guess you don't have this option.
I looked and I did find the two files that 13910634301 mentioned, PslTubingExtract.CATScript and PslTubingExtractTemplate.xls, and these are apparently meant to be used to extract tubing data, which is what I've been trying to determine how to do - this gives me an avenue to explore further, so thanks and good luck on your project!

 

[mschvili]

If you don't have Tubing or Piping Design, the far easiest way is the use points and P o l y l i n e.

CREATE
1. Create you point where you want your bends (coordinates)
2. Press the Polyline icon under 'Spline' in Wirefram&Surface (or GSD)
3. Select the point and enter a radius for every bend.
4. Create a plane at the first point using 'Normal to curve'
5. Sketch profil
6. Create the pipe with the Rib command
7. Shell the thickness

MODIFY
Change the point to modify the corner
The rest modifications speak for it self.

Good Luck!

Matti