Hi all
I have a part (SW18) that does a weird thing on a volume scan:
Attached is the native file.
Do you have any idea what can cause this phenomenon? The outer shape is good
came_int.sldprt
came_int.sldprt
Hi @stefbeno
you must have too small an inner radius
Surface test we go a hair + far
or passed in smoothing ditto we also go + far in surface
@+
Hello @gt22, I don't really see how to do a volume sweep with surface.
In terms of radius, we are 5mm minimum on the grey sketch.
On the captures, the gray sketch is a construction sketch. The blue sketch that drives the sweep is made by shifting (7.5mm) the gray sketch.
Normally, the inner edge of the scan should be coincident with the gray sketch.
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It's quite funny: I reproduce the bug under Sw2020 sp3.0
The problem appears at the beginning of the removal: SW does not even remove all the material at the location of the base body (or drinks the interference in function preview).
Stupid solution but it works : if your pilot curve is interrupted (I did it towards the tool body), then the machining is OK. It can always allow you to make your piece. (the removal of material from the actually circular part does not pose a problem to be carried out)
Even more stupid: if you connect the 2 dots of your previous cut and your profile is reconstituted (with the dot in blue if it wanders or black if you block it), the bug disappears too.
You should send your part to SW support. We may have a correction under SW2025...
General question: is this the first cam you design? Or is it the first time you have this bug with exactly the same method on your other cams?
Nb: after checking your basic external shape is not good either.
Even crazier thing: if you remove one of the 2 bow ends to go back to the initial sketch, the bug reappears......
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Hello @stefbeno,
Totally in agreement with the conclusions of @froussel on the responsibility of the Esquisse4 in the anomaly observed. The two cam profiles generated are false, inside and outside.
The 7.5 mm offset is not to blame, the error persists if it is deleted.
There are two possible solutions to get the right result:
- use Sketch2 as a trajectory in the scan removal function with the cylinder as a tool (image n°1).
- use a sketch as a scan profile, to the dimensions of the diametrical cross-section of the tool cylinder (in red, image n°2), using Sketch2 or Sketch4 as the trajectory.
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Thank you @froussel for this beautiful analysis.
It's quite rare that we do this kind of scanning.
The shot of interrupting the trajectory is a good solution to get around the problem, it is then easy to remove the excess piece.
As suggested, I'm going to open a ticket.
@Zozo_mp: it's attached, unless you want it in step format?
@m.blt :
- I'm not sure I understand your first method: if I use sketch2 as is, my machining won't be in the right place. On the other hand, I modified it to avoid going through the offset sketch and I didn't make the mistake (I hadn't taken the time to try it out before asking the question).
- For the second method (simple scanning), this is the one we have already adopted but we had a doubt if it had a difference in result (it's a desmodromic cam).
Obviously it's the lag that causes the bug.
The result is identical in all three cases:
- with Sketch2 trajectory and volume tool,
- with Sketch2 trajectory and diametrical cross-section,
- with Sketch4 trajectory and diametrical cross-section.
Provided that the diametrical cross-section remains normal to the trajectory during smoothing.
This is confirmed by the comparison of the overview in the three situations.
On the other hand, the same preview using the Sketch4 and the volume tool shows that if the "section" used by SolidWorks keeps the distance of 15 mm, it does not remain "normal" to the trajectory, and the smoothing is not the envelope of the cylinder...
Have a nice day.
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Hi all
Rather crazy thing, if you change the offset dimension of sketch 4 to 7.6 (7 or 8 also works) the trajectory no longer bugs.
There's a damn weird thing.
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