Design Challenge

[ptc-2159145]

I have seen and read threads similar to the one I am posting here, but mine is a little more complex. I am working on a tub design. It drafts outward on the front and back while curving outward on both ends. Think of regular bowl, with flats on the front and back. Modeling the tub isn't the issue. The customer would like to add dimples to the bowl, but still wants to have a straight draw during molding. That means that there cannot be any undercuts when taking a cross section though the dimple. I can achieve what I need though a complex series of surfaces and merges. The process is very involved and time consuming. Does anyone have a simpler solution?
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[ptc-2708796]

I'm not sure this is exactly the same, but I had a similar task to put dimples on a part with a single pull on surfaces that were every which way. What I did was offset every surface the depth I wanted the dimples, set up a pattern of points for the pattern of dimples and create lines from those points in the direction of the pull plane. Then I came back a linear distance along those lines and inserted a sphere and removed material. I wouldn't think this would be that hard on your part because all of the surfaces are tangent and smooth. After the pattern is set up it's just a lot of clicking. Then I went and rounded every dimple. Your task sounds worse than mine because you're coming up a steep sidewall. I would think that an increase in the dimple (sphere side on the sidewall might compensate for the angle, if there's draft on the wall. I'm not sure of how steep the angle you're going up, but it's easy to test a 2-D line at that angle and a circle that has a radius that will cover the whole pull. You can increase the diameter of the sphere, drop the angle so it's less steep, or adjust the depth of the dimples. At worst it should be 1 bottom, 2 front and back, and 2 sides at different offsets possibly, sewn together. If you come at the problem from the single pull plane it's a lot easier than setting the dimples up in a pattern from the side and trying to adjust them. I hope I understood the problem and was helpful, if not I'm sorry.

[ptc-2159145]

Gregory, Thanks for trying, but it didn't work. I tried several different offsets, revolve radii and vertical distances. Either I didn't have the right combination or it is not going to work. Does anybody know of a way to constrian a freeform to a specific sketch? I tried a similar process with the warp but was unable to get it to work as needed.

[DavidButz]

Jon, Do you mean something like this? The tricky thing is getting reference Datums that will pattern properly. The Sketched feature is relatively easy, a centered Revolve of only about 90 degrees. If this is close to what you are trying to do, I can give you more detail. David

[DavidButz]

Jon, A little more detail: 1. Create a dependable surface reference. Even though the inside of the bowl may have been created by one feature (a shell, for example), it's hard to select it as a continuous surface entity in such a way that an intersection or pattern will follow the entire surface. Pick the four surface patches, then Copy/Paste to form a new Surface feature for future reference. 2. Create the OFFSET Plane where you want it, then the blue curve, by Edit/Intersect with the Surface feature. 3. Create PNT0 at some Relative distance. 4. Create A_1 Through PNT0, Tangent to the Surface feature. 5. Create the LEFT_REF Plane Through PNT0, Normal to A_1. 6. Create the SKETCH Plane Through PNT0, Normal to LEFT_REF and Normal to TOP. 7. Revolve a Sketched Feature on SKETCH (A_2 is the axis of the feature) and revolve it about 90 degrees centered on the sketch plane. 8. Group all features from PNT0 to the Revolve and Pattern using the Relative dimension for the Point. David

[DavidButz]

Oops! Step #4 should have said Normal, not Tangent.

[DavidButz]

It would also be clearer if I had used the menu word Ratio instead of Relative in #3 & #8.