I'd like to add draft to all the vertical surfaces of this prop replica, as I am having issues with catching bubbles in a mold with lots of right angles. When I try to either extrude with angle, or use the draft function I am having lots of issues, and not able to get the part to do what I want. I also tried a loft to get there in a round about way, but didn't have luck. I think the numerous small curves are giving me issues. Any ideas?
working with imported curves has MANY pitfalls.
In this particular case, every line segment I checked had a near-tangency condition. cad programs like fusion just don't handle this type of thing well.
you MIGHT be able to unfix the lines and apply a tangent constraint between all the segments
adding constraints-
result after-
that's going to be a real pain.
I don't know what program you used to produce the curves, but there may be settings there to produce a cleaner export, IDK.
draft will fail in areas of high curvature. I can't say for certain that this entire design could be drafted if you re-traced it. However, I did spend just a few minutes tracing one section of the design to see if I could get it to work, and was successful. I was able to extrude it 2 mm, and then apply a draft of 3 degrees to the result (I could not apply the taper in the Extrude itself, and I'm not sure why).
you can see the draft if you look straight down on it:
so, yes, it can be done. It would be tedious, I agree, to re-trace all those shapes, but you could do it, if you were motivated enough. The model is attached, FYI. I would recommend, for the longer shapes, splitting it up into multiple splines, for your sanity, and for performance. Just remember to make them tangent.
@laughingcreek wrote:
working with imported curves has MANY pitfalls. In this particular case, every line segment I checked had a near-tangency condition. cad programs like fusion just don't handle this type of thing well.
I am not sure that this generalization is true. It simply the case that the geometric modeling kernels employed by the different CAD software handle different challenges differently. ASM is very sensitive to the near-tangency problem.
I exported this as a STEP file and was able to draft this entire thing in my other CAD tool in less than 5 minutes.
On the other hand, I've been able to fillet things in Fusion I was not able to fillet in my other CAD tool. And vice versa!
It's a really interesting thing how different kernels handle the different tasks.
@mailjesse where did you go ? Did you give up that easily ?
I was able to draft more than 90% of the shapes to 10 degrees. You never specified the needed draft, so I picked 10% as a rather large value for any form of molding.
The red shapes I was not able to draft past 3 degrees.
The yellow shapes were all good up to 6 degrees.
However, I believe there is also an irregularity or bug with the draft tool. @jeff_strater you might want to look into this.
If all shapes have the same height, then in the top view the base should appear as an equally offset edge when drafted to the same angle. However, there are at least two of these shapes where that is not the case.
In the shape with the arrow on the right side I drafted to 10 degrees, but the base is wider than any of the other shapes drafted to the same degrees.
The red shape to the left with an arrow, I was only able to draft to 3 degrees, yet the base appears more offset than any of the neighboring shapes with a 10 degree offset.
