Help flatting this model

[DuckyB]

I have exhausted all the flatting option I know. I used Catia v5 r20 and went through all the things I usually do to flatten non-intelligent solids and surfaces models.
I also used Solidworks 2010 "convert to sheet metal" command which got me close, but solidworks hates the tips of this part and excludes them form the flatting.
I calculated the bends with my calculator like the old days and came up with 6.3 inch overall. I milled the flat pattern and the brake guy formed it, then CMM bought the part off.
But I’m wondering why it never flatten using the cad tools we have. Can someone try to flatten this part please? I really want to know what you some up with.
Thank you


John B

 

[prolynx]

In the generative sheet-metal design workbench, I did it with a hopper, as the "recognized" command was complaining about thickness not being constant on the part (there is at least one panel with a different thickness). First extract the surfaces with tangent continuous (at first also correct a tangent problem on one of the tip), then "hopper" and voila. I got a bit over 6.4 inch overall, because I used Catia default parameters for the K factor.
But why not do this directly in sheet-metal workbench ? You could do this directly with an extrusion for instance.

Sebastien

 

[DuckyB]

Anybody? Boy its quiet in here.....

John B

 

[DuckyB]

Sebastien,
I always for get about the hopper. Thank you for the step by step.

Yes the thickness not being constant is a issue on lots of parts we receive. I usually use the Generative shape design-> extract function and generate a constraint thickness using the Part design-> Think surface command.

John B

 

[prolynx]

I rarely use the hopper command, as it's a bit unstable if I do changes up or down the tree, so maybe if you can, you probably should try to fix the geometry first to have constant thickness and use the "recognize".

Sebastien

 

[DuckyB]

Sebastien,
Great I came up with 6.421. Thank you for your help, I learned a lot.
What steps did you take to correct the tangency errors?


John B

 

[prolynx]

I simply just edited the sketch and added the missing tangency constraints. The lines seemed almost tangent, but not tangent enough for Catia

 

[DuckyB]

Yeah I dont use Catia for drawing or repairing models, just getting annotaions and flatting out sheet metlat parts when needed. I would like to know how you added the missing tangency constraints if you dont mind.

 

[DBezaire]

If it is a solid with history
Edit and constrain the geometry in the sketch. I would start with dimensional constraints then move to tangency constraints.
If you are using GSD
Try joining the surface data and play with the angular tolerance. You can also turn on the check tangency option to show the problematic areas. If the angular threshold in Join does not tweak it enough you can use the Healing command on the problem surfaces.

If you have access the HA (Healing Assistant) module, you could heal the internal patches of a larger join.

Regards,
Derek


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