I have to make an impression, on a cylinder, which follows a helical trajectory then a "turn" and again helical parallel to the first.
I make a closed sketch of the edges of the impression, which I roll up on the cylinder.
I make a sketch of the shape of the impression on the end of the cylinder.
I carry out a sweeping material removal, with the form sketch using the winding as guide curves.
And that's where it crashes... If I just do the beginning of the trajectory (first 2 segments) it works. If I ask for more, it sometimes works... To summarize, the behavior of Solidworks is random.
After multiple attempts I have at best half of the trajectory (helical go + turn but not the return).
The question for me is, is this a limitation of Solidworks' capabilities, or do I have a hardware configuration problem that does not allow the function to be resolved in a stable and reproducible way.
If I understand you are in the case of a double thread screw with a stock termination that allows you to use one thread for one direction and the other thread for the return while the screw always rotates in the same direction.
In other words, the equivalent of a swerving screw but without a cross thread
If I understood the part correctly, it is enough to make two helical grooves with a large pitch so that the return helix can fit into the space left by the coil of the outflow.
So it all depends on whether you are building in one piece or if you are doing it in three parts. I don't see where SW's limit would be. If I understand it's because your guide curve is not continuous and that the sweep removal function doesn't like it at all (also if the angle of the turns is too tight). If that's all the problem, your guide curve must be made in one piece Just use the ==> spline ==> spline tool==> adjust the spline.
You just have to know that it works even if there is no spline, for example a radius is a straight or curved line. It's a poorly explained function perhaps.
We should just specify a few points as well: 1°) Are you doing kinematics in an ASM with this part. 2°) there is the equivalent of a finger nut that should slide but there are also loss of contacts when you run the kinematics.
Does the profile swept to make the removal greatly exceed the volume? Sometimes it gets stuck because we find ourselves side by side and it crashes. Removing too much material can be a solution.
There should also be options for the rotation of the section (mandatory to put something given the shape to be made).
You probably also need to use a guide curve to really manage the orientation of the sketch throughout the scan. It's painful but you probably have to do almost the same curve again but offset.
Another method to test: instead of doing a material removal, you do a sweep by creating a body that is not fused to the 1st that you then subtract with the Combine function. Sometimes this method is faster.
That's what we told you in one of the posts: the turn is too abrupt, you should put a second guide curve just for this part. And if you want it to work perfectly, put two circles (profile, sketch) at the beginning and end of the turn. You can also increase the radius of the bend a little because of your application, it shouldn't bother anyone. Especially since heating cords also don't like too sharp turns because it inevitably causes overheating in these places and cracks in the long run. This is because the electric current takes the shortest path in bends and does not follow the neutral fiber. Solidworks thinks a bit like if you try to bend a copper tube by hand, because the material is not stretched, it creates folds. The double guide curve gives a result equivalent to the bending machine.
Yes, changing the guide trajectory too abruptly is not recommended. Another tip to avoid errors in the removal of material due to tangent faces, try to make sketch 3 protrude outwards.
Ok for the radius at the beginning, which is bound to disappear anyway in the rest of the construction of the part, but it also doesn't follow the curvatures of the half-turn at the end of the cylinder. And the spokes cannot be changed.
As we already mentioned the colleagues, it is preferable to drop the operation in several operations (propeller part / loop part) because when a trajectory becomes too long SW tends to do strange things like cutting turns for example.
Have you tried the option to remove a volume body (3rd tick always in the same function)
You must first create a disjoint volume body that would correspond to the tool that would remove the material and placed at the starting point of your scan profile
Here's how it looks with the preview on a single propeller
and here is the body obtained
I know (from having encountered the problem on cams) that in terms of real machining, there is a difference between the scanning of a section and that of a volume: the volume is more faithful to reality.
Indeed, the removal of material by a volume works very well.
To make the helical trajectories, no problem... but with the U-turn that makes the junction between the 2... that's where it gets complicated!
To make this part I have a helical + half turn with the method presented in the initial message and the return with a removal of material by a volume. The problem is that the junction between the two is not clean...
