new test (the representation of the removal of material is not easy since indoors...)
Based on the same principle as the previous test but the cylinder is made in two stages (before and after winding)
Note: Pay attention to the orientation settings of the profile in relation to the trajectory for ovals ...
That's a good idea. First of all, it allows you to see what the scan looks like.
A very stupid thing about its sweep is that it rotates.
So you have to put the options that allow the tool to always point to the center along its path. If the tool has a fixed direction it will crash. Bring a long enough tool too (you don't have to be right tangent but protrude inside the cylinder)
Maclane thank you for taking your head on a Friday ^^ so for your last rendering yes but no 
when I say that it's inside the cylinder it means the same as what you did on the outside side but in the inside and not in the cylinder 
but I appreciate the effort ^^
Hello
In my example, the smoothed pickup refuses to work if I try to use the edge (?) generated by the winding feature as a trajectory.
On the other hand, it works by using a (composite) curve as a trajectory, a curve created on the features of this edge...
What is the shape of the abduction section?
Hello
I can look at this side although I have never used a composite curve yet.
The section is an oval. 1.6 wide and whose farthest edge is also 1.6 from the center which is at the point of meeting with the line
Arrg! Maximum effort...!!
It's " funny " Solidworks refuses the scan if the trajectory sketch starts directly on the cylinder (I had to create an artificial departure offset)
Part4.SLDPRT (1.4 MB)
it seems to correspond to what I need but I can't grasp the story of the artificial shift :s (Friday for everyone XD )
My 3D sketch is a " conversion " of the result of the scan, it is this sketch that I use as a trajectory in the scan, If I leave the sketch as it is, the sweep is not done but if I extend my two start and end lines outside the cylinder then the sweep is accepted...
(I think Solidworks also understands that it's Friday at the end of the day... he is probably tired.).
if I understood correctly → 3D sketch ->selected the winding plot → convert the entities and extend the 2 starts? Because if that's right, it works for me 
I extended the starting points and created a plane on one end to model the sketch of the shape to be scanned.
I can't do it aaaarrrrgggg well I'll do it again on Monday with a rested head.
First of all, thank you to everyone so far^^
Hello.
Sorry for my somewhat " boaty " question... but how thick is your piece?
Hello
Maclane: So, I've tried your method several times but I can't understand why, when I want to apply, it doesn't work. Each time I get the message " the scan operation has not been completed."
Coin37coin: so the part is 6.5mm thick for a material removal of 1.6mm so I'm wide normally
Normally yes. It's a trompe l'oeil effect then 
It's okay I succeeded \o/
In fact it obviously came from the fact that in my winding function, I used a spline...
So I used Maclane's method but kept the 3D sketch in " line " mode and not spline for the material removal guide and it was done.
So I take note that in more complex functions, you have to avoid splines...
Many thanks to everyone and especially to Maclane who allowed me to have the click 
… pfff all this for that!! 
Glad you managed to find the solution.
Personally I didn't think about splines for the good reason that ... I avoid them like the plague (and Covid, to a lesser extent). It just goes to show that on Monday, we have clearer ideas. 
As you say, all this for that big thank you in any case
Hello,
I just did the test under SW2019 and I don't have any problem, just pay attention to the orientation of the constrained " oval " towards the center of the cylinder. which must not have been the case on the Maclane capture where we see the entrance and exit with a different orientation. No need to make a staggered start either.
I'll put you this version if you want to compare. Everyone must be able to open from 2019
REMOVAL OF HEATING CIRCUIT. SLDPRT (1.0 MB)
thank you very much I'll take a look at it
