Hi, I am sure many of us have encountered this problem and may be there was already a lengthy discussion about it before. I hope to learn more about this issue from all of you.
Whenever creating a sweep feature along a closed contour, using "trajpar" parameter in its section will fail the feature most of the time. The questions are:
1. reasons of failure
2. does this happen also in Creo 3 or even Creo 4?
3. What really annoy me the most is it does not fail ALL the time, sometime it just works fine. I have an example here:
The first feature works well. The 2nd and 3rd features differ only in dimensional scheme and this made a huge difference ! I attached here Creo 2 file so that you can play with it and please share what you find/learn from it. Thanks in advance.
For me, failures like this are often affected by part accuracy.
I've never come up with a universal cure.
Try using absolute accuracy so calcs don't change if the part bounding box changes size. Then try making the accuracy value a little smaller. That's usually the direction I start.
I once tried to make an animation of a sweep that used a datum curve by equation. The trail file increased the angle around a circular path and then made a JPEG image. It would increment and repeat the process. It failed at random angles and sometimes would work if the accuracy value was smaller and sometimes require it to be larger. No matter what setting was made the sweep would fail at some other point in the process.
When I try this it appears it's related to the type of dimension created in the section. For me it seemed:
1) a linear dimension was okay for one direction only for a dimension across the width of the section (still caused failures)
2) linear dimensions in both directions seem to be good if created from the centerlines to one of edges of the section
3) create radial or diameter dimensions in both directions (can be done by selecting weak dimension, RMB, covert to radial or diameter)
4) create diameter dimensions by using the edge-centerline-edge selection method
2), 3), and 4) seem to be the best methods to dimension the section.
This also can be a problem - the dimensions have to be able to follow the geometry as it turns. If a dimension is locked to a horizontal measure or vertical measure the section can fail. I skipped the possibility because it should be obvious. It can be diagnosed by making changes such as making the multiplier to the angle less than 1 and increasing it until the dimensioning fault is obvious.
I can't see the either sketch well enough to see how the sketch items are constrained.
The second centerline is perpendicular to the first, the long sides are parallel to the centerline controlled by the angle with one of the lines having a symmetric constraint, the short lines are parallel with one perpendicular to one of the long lines also with a symmetric constraint. Changing the dimension types worked for me. in another file they posted which appears to be constructed the same it appears to want dimension defined as linear but doesn't like them as radial or diameter dimensions. The only other thing is the geometry is in mm so the trajectory is 10 mm in diameter and the section is 3 mm X 1 mm.
Thanks, I will try with different accuracy seetingto see if it makes any difference. We have a standard accuracy setting that I need to stick to but i will play with it to see how it affects this feature.
This is pretty interesting. For different section geometry, it's quite hard to determine what to or how/what not to dimension other than trial and error .
Got some reply from PTC, not much different from what you guys already shared/knew :