I need to draw 2 overlapping helices - one clockwise and one counter-clockwise, then sweep a circle along each helix. I had to use datum planes normal to helices at their ends and that forced me to mix Part Design and Part workbenches. It seems to work but there are "Part has null shape" errors associated with the datum planes and I can't use Part Fuse on those bodies. Should I do it in a different way (assuming that TNP is not relevant in this case and thus all approaches leading to the working model are acceptable) ?
Please excuse me if I am misunderstanding the problem.
Why do you need the datum plane from PD and circle from sketcher?
You have made the helix in Part. Could the circle also not be made in Part? Then change its map mode and use the end vertex of the helix as the first selected point (to get the centre of the circle in the correct place), with the helix edge as second reference (to get the circle pointing in the correct direction). Sweep the circle along the helix.
Workshop_Notes wrote: ↑Wed Jun 07, 2023 6:35 pm
You have made the helix in Part. Could the circle also not be made in Part? Then change its map mode and use the end vertex of the helix as the first selected point (to get the centre of the circle in the correct place), with the helix edge as second reference (to get the circle pointing in the correct direction). Sweep the circle along the helix.
Thank you very much. I just had no experience with mapping (I'm still more used to the traditional datum and sketch-based approach known from other CAD software). This works great but I still can't apply Part Fuse to this properly. Isn't it possible to merge those two swept geometries ? I also need to pattern them but I'd like all the wires to be connected.
... The arrays should form a single body:
My problem is:
using circle as cross section => artifacts in display appear
using e.g. a square => no artifacts
in Helix sweep and in Sketch_On_Surface (CurvesWB) sweep
hammax wrote: ↑Thu Jun 08, 2023 2:33 pm
... The arrays should form a single body:
Thank you very much but after exporting to step and importing to FEA software, I get 50 separate parts. Is there a way to merge the wires so that a single continuous part is exported ?
hammax wrote: ↑Thu Jun 08, 2023 2:33 pm
... The arrays should form a single body:
My problem is:
using circle as cross section => artifacts in display appear
using e.g. a square => no artifacts
in Helix sweep and in Sketch_On_Surface (CurvesWB) sweep
Yeah, there's a nasty visualization issue causing the distortion of sweeps based on helices: viewtopic.php?f=3&p=551278
Unfortunately, adjustment of tesselation settings doesn't help in this case.
NewJoker wrote: ↑Thu Jun 08, 2023 5:16 pm
Thank you very much but after exporting to step and importing to FEA software, I get 50 separate parts. Is there a way to merge the wires so that a single continuous part is exported ?
What happens if you set Fuse = True in the array properties?
NewJoker wrote: ↑Thu Jun 08, 2023 5:16 pm
Yeah, there's a nasty visualization issue causing the distortion of sweeps based on helices: viewtopic.php?f=3&p=551278
Thanks for finding out that the problem has occurred before.
If, as suggested above, fusing works with a square, could you try a many-edged polygon to fake your desired circle?
In your original example, I found that if you reduce one of the helices from 16mm high to 15mm high (so there are only two places they intersect), it is possible to fuse them. I also tried a few random left and right helical sweeps and they fused OK. It must be something quite specific to the geometry you have.
Workshop_Notes wrote: ↑Thu Jun 08, 2023 7:08 pm
In your original example, I found that if you reduce one of the helices from 16mm high to 15mm high (so there are only two places they intersect), it is possible to fuse them. I also tried a few random left and right helical sweeps and they fused OK. It must be something quite specific to the geometry you have.
That's interesting. I wonder if it can be considered a bug.