I'm trying to model a sheet metal part with a flange around its perimeter. I already have radial profile geometry including the flange. I created a Flange around a continuous perimeter, but it will not unbend correctly. Does anybody have a suggested approach?
Creo sheet metal will only work on non-intersecting bends. You have to think of bend only with a press brake. Straight bends that don't intersect at all.
The deformation (stretching or bunching) in rolling an item like that is not straight forward.
I am getting closer to a solution. I was able to create the bend the u-shaped profile but the part didn't match the original shape.
The interior surface of the finished part should line up with the green profile. Any suggestions to fix the problem?
How did you construct the original shape and how did you do it differently than the solid?
This should be simple. Creo 2.0 attached
BTW: The drawing and dimensions are not the same in the hand-drawn drawing.
There is also an over-constrained condition that cannot exit.
Thanks for your feedback. Unfortunately, some legacy drawings can't be modeled as published. I show over constrained dimensions (reference) only to validate hand drawing.
Your curve profile is not the same (fewer arcs and different dimension scheme for arc centers) which could factor into the simple solution.
Not sure what I am missing.
Maybe I understated the level of effort required.
The drawing is wrong, no doubt! Someone is trying to make a drawing based on a defined flat blank.
Suspect dimensions are the 72-1/8 and the 1-7/8.
I did get everything to match if I let the 1-7/8 float but I doubt this is the shape that was expected.
As to the "means" of getting there, this time I use an extrude. Sweep would have worked similarly.
I did have a to make a few assumptions since the drawing is not published complete: IBR=T and T=1/8"
What I did was to use the non-tangent specified dimensions and overlaid it with a spline. This manages both the requirements and the transition tangents.
Also note that this is certainly not the highest level of integration.
I did some iterations to get the numbers to match (IE: 72-1/8 is slight short, 5.72 may not be exact).
With a little more work, you could make this fully parametric based on a flat-pattern so you could easily define more versions with the same model.
Edit: Also consider the fact that the flanges on the edges will change the K-factor of the bend. I've left it at default. The actual K-factor value will change the shape slightly. This is normally determined by process and experiment.
Awesome solution TomD!
You are correct about suspect dimensions on the print. My approach was similar to yours but I didn't adjust my model accuracy. I opened your model and experienced similar failures with default accuracy setting. Made one adjustment and solved the problem. Opened an early version and problem solved...I need to re-sharpen the saw!
Thanks for hanging in and walking me through.
Interesting that you needed to change your accuracy settings. I left the default accuracy of relative and .0012.
Darn, I forgot, yes... when you open a new sheet-metal part, the accuracy is set much tighter.
If you convert a part -to- sheet-metal, it maintains your default accuracy for solid PRT files.
Glad I could help, Adrian. It is an interesting challenge.