Parametric Circumferential Layout

[snufflufikist]

Hi,

I am attempting to create a part/drawing in Pro/E based on an
AutoCAD drawing. The part has 20+ holes and half holes around its OD.
It's quite easy to model the holes using a table pattern (patterning the
diameter, angle to front plane, and distance from end of part).

However,
to show this in a drawing is another matter altogether. Rather than
have 12 cross sections to show where every hole is located, the AutoCAD
drawing had what is referred to as a "circumferential layout". It has
the OD of the cylinder "unwrapped" and the geometry is shown using the
same 3 dimensions (diameter, angle to front plane, and distance from end
of part).

To do this in Pro/E using the methods I am familiar with presents a few problems:
-
if I draw a sketch, wrap, and cut into the cylinder with it, it's
awkward because my sketch covers 360

 

[krow72]

you can create the tube with the holes, turn it into a sheetmetal part, create a "rip" for a seam and then unfold.

 

[cpoirier]

I see the part is not a sheet metal part by the lower left view, partially obscured.
This seems to be a machined part, the flat layout can not be done in Pro automatically. It would be nice if it were possible to define a curved cross-section and have pro e flatten it, but alas this can not be done. You can design the part, copy the surface and flatten it, but the holes will be ovals when flat if they are machined when in a tube shape. You need to do this the hard way to be correct and section the hell out of it. A cylindrical hole table could fit the bill, but god knows how to coax pro to do this or if it could be done. Any takers on figuring this one out as a challenge?


Chris

 

[snufflufikist]

You are correct Chris, it's a machined part.

This is one of the simpler parts. The others I have contain slots with strange and wonderful angles (jay slots to be precise). I've had a lot of trouble with them in the past in terms of model robustness.

My current workaround approach is to build two models. One is the actual cylindrical part which will be used in the assembly. It is modeled using a pattern table which is very easy to make. The other model is a flat sheet whose length is equal to the cylinder's length and whose width is equal to the cylinder's circumference. I have set up relations so that all dimensions are tied to the cylinder circumference as (ANGLE / 360 * circumference). To edit the hole positions, the next person will have to edit the ANGLE "variable" in the relations.

I created my drawing using both models. I've had to do the angle dimensions (as ordinates) manually. I figure even if the geometry isn't accurate on the section view (left above), that's ok because it's fudged on the AutoCAD version anyways. The important part for the machinist is the circumferential layout.

It's working decently for this simpler part. I think for the others I will be using the toroidal bend and just accepting that the model is a bit inaccurate and that the angle dimensioning is manual. Still interested to know if there is a better way! Thanks for the replies.