ProE Degenerate Segment Failure

[TedJ1]

Can anyone please tell me why I get the following error when I attempt to change the offset of POINT0 along the datum curve from 0.05 to 0.25? I'm using Pro/Engineer Wildfire Student Edition.

"Feature #8 (PROTRUSION), PART SPUR_GEAR_TESTB, failed regeneration. Section regeneration failed. Degenerate segment encountered."

The part file can be found at this link:

http://www.afafa.org/Unlinked/spur_gear_testb.prt.4

Thanks so much. If you can help me to solve this problem (before Pro/E drives me totally bonkers), I'll send you a $50 check.

Thanks,
Ted

 

[markthemech]

The problem is in the sketch.





"Degenerate segment" is Pro/E's
way of saying it doesn't know how to do the math to calculate the shape
you need. It happens when an entity in a sketch is reduced to zero size
due to the dimensions and constraints you've applied.





It also
happens, as in your case, when the sketch itself has references to
geometry that isn't always available. I see what you tried to do by
having the pattern increment the point on curve, but the skecth still
references front and top. Once the sketch hits the other sides of these
datum planes, your original dimensioning scheme falls apart.





I fixed the part and uploaded it tohttp://www.mooload.com/file.php?file=files/1133100613/spur_gear_testb.prt.5






It was fixed in WF2 Student. If you are using WF1, here is what I did:





1) Made an axis through TOP and RIGHT. Reordered it to before the group.


2) Made a datum plane through previous axis and the datum point.


3) Ungrouped G1.


4) Reordered datum plane to before the protrusion.


5)
Edited definition of protrusion. Changed the Sketch view reference
plane to the new datum that you have created (2nd reference), and made
it point to the Top of the sketch.


6) Chose Sketch-->References,
deleted references to all datum planes, and then added a single
reference to the new datum plane. Also deleted reference to the datum
point.



7) Use Constraints (Align) to ensure that the centerline of the gear tooth is aligned with the new datum plane.


8) Made one more dimension to denote the width of the tooth at the top.


9} Completed sketch.


10) Hid new datum plane.


12) Regrouped point, datum plane and protrusion.





This can now be patterned just fine.





Send the $50 cheque to the Red Cross.

 

[TedJ1]

Hello Mark,


Thanks for responding. Unfortunately, I could not open the part file. So, I followed your instructions (precisely) without problems up to step 5. At that point things become unclear. I choose 'Edit Definition' then press the Sketch button. In the Section dialog containing


Placement


Sketch Plane


Plane []


Sketch Orientation


Sketch view direction (Flip)


Reference []


Orientation [Right V]


I attempted to reset Reference to the new datum plane that I just created. But ProE doesn't allow that.


According to your instructions, the new datum axis is equivalent to the line of intersection between the Top and Right planes. Is that right? Then the new datum plane, in order to pass through both the new axis and the existing datum point must be equivalent to the Top plane. But that isn't correct, is it?


I really appreciate your having taken the time to look at this

and I apologize for my inability to follow through to successful conclusion, but could you please tell me how I have misread?


Thanks again,


Ted

 

[TedJ1]

Mark,


Ok, I figured it out. I believe what you meant to say in step 1 was 'Make an axis through FRONT and Right' (not Top and Right). Changing that step makes the rest possible.I'll study the solution carefully to better understand ProE's needs in the future as my mistake, as you know, was fundamental.


BTW - As far as charities goes, would you mind if the donation goes to a Hurricane Katrina relief fund? I gave $2000 to the Red Cross after 9/11 and was disappointed to hear of their rather large percentage of funds not going directly to the charities intended for. But hey,your call.


Thanks so much!

Ted

 

[markthemech]

Absolutely! As long as it is going to someone who needs it.



A couple of things to note about the problem you've had:



This is the way you pattern sketched features radially using Pro/E
(prior to Wildfire 2.0). The idea is that pattern regenerates
instances, it is using the exact same sketch over and over, except it
is being rotated. WF2 has an Axis pattern tool that makes this a lot
simpler (I avoided the simple "use the axis pattern" response since I
wasn't sure).



Something you may also want to consider: You may have a reason to
pattern the feature using the point on datum curve technique, but an
alternative would be to create the datum through the central axis and
offset at an angle from FRONT. Having this in the group with the
protrusion would allow you to pattern it by an angular increment (=
360/# of instances.)



Good luck!

 

[TedJ1]

I'm not sure how to determine the Wildfire version that I'm using, but I'm glad that you took the long way.


The reason why I used the point on datum curve technique is because I kept having difficulty with angular flipping when I would reference the part to an anglerelative to the Front or Right plane. I.e.the part jumping180 degrees apparently randomly, which I could think of no good way to control. Point on datum curve seemed the only way to provide an angular lock. Perhaps your solution inherently solves that problem already. If I find time, I'll investigate that.


Thanks.


P.S. I made that donation. I thank you. The Red Cross thanks you. We all... thank you.

 

[markthemech]

You can see your version and build code under Help-->About Pro/Engineer



This is something that new Pro/E users commonly have a problem with.
I've been teaching that to people for the past 4 years... At least
until the axis pattern. I still show the method to demonstrate an
alternative to the axis pattern, in case it doesn't work.



The part that a lot of people don't get is that datum planes have
"positive" and "negative" sides, so once a sketch with angular
dimensions wrt datum planes regenerates beyond 180, the dimensions
"flip" sides and everything falls apart.



Using the patterned datum plane provides a "moving" horizontal reference for each sketch in the pattern.



Edited by: markthemech