Problems creating rounds??? Creo 2.0 M120

[A.DelNegro]

I recently updated to M120. I have noticed today that I have been unable to create a round in the simplest of corners. Has anyone else had this issue? (I can’t say for sure if it has anything to do with M120) If I increase the radius, it seems to be ok, though I would think this would be a more complex round to construct. I just want a 1/8” round. I’ve never seen anything like this before, so I’m really stumped. Earlier I was trying to round the outside corners of a plate and had the same issue. Thought maybe it was a corrupt part. Now its happening on this one too.

[cid:image001.png@01D005A6.450B1A90]
[cid:image002.png@01D005A6.C4914870]
[cid:image003.png@01D005A6.C4914870]

Tony



I get these errors in the Troubleshooter…

Set cannot be constructed on the highlighted pair of surfaces.

Recommended actions:

Try to start from different pair of surfaces. If necessary,
try to create feature as "Unattached", and complete it using quilts,
or try changing the dimensions.

And…

Could not construct feature.

This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

[bgruman]

Hmmm, That sure looks simple and I'm not on M120, so you may have
something else at play here but...
Whenever I have trouble with a small round, I look to the model accuracy.
Tighten up the accuracy, and the round will usually go on.

Good Luck
Bernie

Bernie Gruman
Owner / Designer / Builder
www.GrumanCreations.com


On Fri, Nov 21, 2014 at 3:18 PM, Tony DelNegro <->
wrote:

> I recently updated to M120. I have noticed today that I have been
> unable to create a round in the simplest of corners. Has anyone else had
> this issue? (I can’t say for sure if it has anything to do with M120) If I
> increase the radius, it seems to be ok, though I would think this would be
> a more complex round to construct. I just want a 1/8” round. I’ve never
> seen anything like this before, so I’m really stumped. Earlier I was
> trying to round the outside corners of a plate and had the same issue.
> Thought maybe it was a corrupt part. Now its happening on this one too.
>
>
>
>
>
> Tony
>
>
>
>
>
>
>
> I get these errors in the Troubleshooter…
>
>
>
> Set cannot be constructed on the highlighted pair of surfaces.
>
>
>
> Recommended actions:
>
>
>
> Try to start from different pair of surfaces. If necessary,
>
> try to create feature as "Unattached", and complete it using quilts,
>
> or try changing the dimensions.
>
>
>
> And…
>
>
>
> Could not construct feature.
>

[mlocascio]

Tony,



Is there any kind of order of operations issue here? It seems to me like what you are having trouble with relates to an order of operations scenario. Also, I don’t know if I can assume that there is enough “land” for that 1/8” radius on the inside. If you go surface to surface it will give you a different result.



Mike Locascio

[A.DelNegro]

I’m not really sure what the problem is. Some pointed out the accuracy. This should not be an issue since I’ve made hundreds of parts with the same start parts without issue. Also, the radius is NOT too small. As you can see from the handles in the first image I sent that the 1/8” dim is about half the width of the shortest shoulder.

I did find this…

[cid:image004.png@01D008B9.5BC9ACE0]

If I click the “extent surfaces” button, the rounds form just fine. I’ve never had to click this, and I do not recall changing anything in the config.pro that would affect this. Is the default to have this clicked already? Any clues?

Thanx
Tony

[c128]

Hi Tony.

From the screenshots I guess this part is not top-secret... Would you consider uploading it? Might make it easier to check what's wrong or test it in other maintenance releases.

Regards

Matthias.

[A.DelNegro]

The part is not top secret but I tried something to test the system. I created a part using my default start part that has been around since 2008 and then created one with no start part. The one made with my start part has the issues, the new one doesn’t. I would think the file might be corrupt, but as I said, the start part has a rev date of 2008 and I’ve been using it since then without issue. The weirder thing is that I opened a files that its about 1 year old, and it doesn’t seem to have the issue.

I’ve attached the one that has problems. If anyone can open it and get the rounds to generate in an earlier version of Creo 2, this could narrow it down.

Thanx
Tony

[rrich]

I opened it and had to go to edit definition on the first round and it fixed it. Then I edit def on second round and some ref is missing on set 1 if I remove set 1 it works. If I replace edge in set 1 it works.

Creo 2 m40

[jmoody-2]

The second round tries to round an edge that is rounded by the first round; I just deleted that set.

Increasing the tolerance allows the rounds to complete e.g., from 1e-6 to 1e-5. (M110) Unless you have a reason, an absolute tolerance of 1e-6” on a 5” part seems extremely small to me.





John

[TomU]

I think something else is going on here. Increased accuracy shouldn’t cause this round to fail. I decided to try this in Creo 3 M010. Same issue.

I then created a brand new model from the PTC’s own start part, created an extrude 5x5x5, and set the accuracy to .000001. Same issue. The default round value (.11) fails, and the intended value (.25) fails.
[cid:image002.jpg@01D0098D.E9307490]

Interestingly, if you change the round type from rolling ball to “Normal to spine”, it’s perfectly happy.
[cid:image006.jpg@01D0098D.E9307490]

I think this needs to go to PTC. I’m more than willing if no one else already has.

Tom U.

[TomU]

PTC tech support has confirmed the issue. See CS191895<">https://support.ptc.com/appserver/cs/view/solution.jsp?n=CS191895> or SPR 2249445<">https://support.ptc.com/appserver/cs/view/spr.jsp?n=2249445> for more info.

[cid:image001.png@01D00ED5.499E2BF0]

They left it “medium” priority (which is really low) because there are multiple workarounds:

In Creo 3.0 M010, the reported round with a radius of 0.105 could be created successfully, if the round is defined using any of the below mentioned options. However, the round can be created in WF5 using default settings without using any of these options.

a. Use “Normal to spline” instead of “Rolling ball” OR

b. Use “Extend Surfaces” OR

c. Use ‘Chordal’ option.

Tom U.