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Problem with a round feature

MarkEvans
1-Newbie

Problem with a round feature

Hey all...I am having a problem with a round feature in a part I am designing. In short, the feature keeps failing and I can't figure out why. I've attached a copy of my part. Refer to 'Round 7' in the model tree. If you can figure out how to make this work, please let me know. Thanks.


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1 ACCEPTED SOLUTION

Accepted Solutions

Here is your part, I believe finished.

I assumed you're cutting the ribbing with a ball mill so I modeled accordingly

As I mentioned earlier, I reordered some features, eliminated some double definitions and only added one additional feature. - round 8

The sketch that failed on me was missing the sketch plane definition.  as soon as I selected the correct plane, all else worked.

enjoy

View solution in original post

10 REPLIES 10

Mark,

I think you cannot create Round as Solid feature. Create it as Surface and close the space between round and model geometry.

round.png

MH


Martin Hanák

first, I switched trajectory ribs

I then moved failed feature - round 7 - under rib 2

created a new fillet (opposite of round 7)

went into feature round 3 and removed the duplicate definition of round 7 and new fillet

now it fails at sketch 2 and I don't have anymore time to play with it

That won't work if there's draft.

Makes it easier then!  Unfortunately, everything I've had to do for the last 4+ years has draft everywhere,  I can't open any of these files so I can't tell if there's any or not.  Which is why I said "if".  Ah well, but that's what makes designing IM plastic parts so "fun"! 

JamesAvis
13-Aquamarine
(To:MarkEvans)

Add a small extrusion to create a continuous surface at the top, first.

9-24-2015 3-00-01 PM.png

Then the round will solve itself.

9-24-2015 3-01-49 PM.png

Change the transition stop case...

Click on the red highlight at the top of the preview and the options will be available.

stop_case_rounds.PNG

I wasn't sure if you were trying to get a controlled radius or a full round to the center boss.

Either way, the software is a bit finicky on the second instance.

Creating both rounds in a single feature makes this work.

The video will show how I was struggling to get either possible results.

Video Link : 6359

Thanks Antonius...I tried this approach too and it worked great. It's a little cumbersome but seems to work just fine.

Here is your part, I believe finished.

I assumed you're cutting the ribbing with a ball mill so I modeled accordingly

As I mentioned earlier, I reordered some features, eliminated some double definitions and only added one additional feature. - round 8

The sketch that failed on me was missing the sketch plane definition.  as soon as I selected the correct plane, all else worked.

enjoy

Thanks Ron. I hadn't tried re-ordering features in the model tree but this definitely did the trick.

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