Referencing curved surface for extrusion

[newman180]

I'm new to CATIA V5 after using Pro/E, Solidworks, and UG.

What is the best way/tool to create a bracket which connects to a curved surface which has no data attached? I can't seem to figure out how to do this with a solid, but especially with the sheet metal tool.

I have been trying a few different methods with using the boundary and extract feature, but I feel I am missing something.

Please let me know if more information is needed.

Thanks.

 

[jackk]

can you provide a picture of what you're trying to create?

 

[newman180]

Here is an example. I have a plate floating between three cylinder sheets. I need the plate to bolt to the curved sheets. How do I make the interface for the plates mounting points to follow the curvature of the cylinders?

Does that make more sense? I was reading that maybe I could extrude through the surface and then use the split tool?

 

[jackk]

Thanks for the picture!

To do this with Part Design: First, modify the plate sketch to extend the plate to the inside of each cylinder (or add smaller tabs). Then Split the plate with one cylinder to get the curved edge. Use that edge to make a Pad (Thick option active) going up or down along the cylinder. Finally, add inside and outside bend radius. Repeat for the other two mounting flanges.

You could do something similar with the Aero Sheetmetal workbench (not the standard license) since those flanges have curved bends.

 

[newman180]

Thanks Jackk. I will try that!

Can that be done in the sheetmetal workbench?

Is there an advantage of using the sheetmetal workbench over the part design if I am making a thin bracket?

 

[itsmyjob]

You can do it with Generative Sheetmetal (it's tricky but not impossible). Would I do it?
It looks easier for me to use Sheetmetal in this case, I would give it a try...
I also understand the limit of catia with deformed parts and flat pattern (CATIA is not 100% accurate)

Eric N.
indocti discant et ament meminisse periti ​

 

[itsmyjob]

the trick in this case is to make a swept on the edge curve and not to try to make a wall & bend

Eric N.
indocti discant et ament meminisse periti ​

 

[jackk]

Some of the advantages to using Sheetmetal vs Part Design vs GSD are:
- automatic uniform sheet thickness
- automatic bend radii
- automatic bend reliefs
- sheetmetal features (stiffners, flanges, jogs, etc)
- checking for producibility
- and the biggest advantage is flat pattern development

I disagree with Eric's recommendation to use Generative Sheetmetal. My understanding is this package will only flatten straight bends (parts that are formed on a Brake machine). That's why I recommend using the Aerospace Sheetmetal package since this part has curved flanges.

http://www.3ds.com/products/catia/p...t/ASL/?cHash=8709f69ae2a260ffb55d096e2e7a7318

Eric: were there some recent improvements to the Gen Sheetmetal workshop?

 

[itsmyjob]

I just said I would try GSM over PartDesign. I am sorry if you misunderstood me.

We do not have Aerospace SM as we do not have a business case for it ($$$$).

I fully understand Aerospace SM could give a better result in developing bend on curve as compensations are available.

With R20 we do not need DL1 no more to work with non ruled surface (Surfacic Hooper). But as I said and you confirmed GSM is not very good with that, this is the limitation I was talking about.
We can create Flange on curved edge... this is the trick we use to avoid the cost of AERO SM. See attached picture.

I do not know if AERO SM is keeping symmetry on flattening non ruled surface.

Eric N.
indocti discant et ament meminisse periti ​