Fully defined sketch not redrawing correctly after dimension change.

[Anonymous]

Having an issue with sketch objects not redrawing correctly after changing a user defined parameter. The parameter changed isn't used in the sketch, but it changes the position of the geometry that was projected into this sketch and then changed into construction lines (RaspberryPi board outline that two other parameters control the distance from the left and bottom edges). With the 10mm change the added mid point construction line (used for mirroring) moves with the projected geometry, while with a 20mm change it doesn't. With a 10mm change the sketch moves with the projected geometry and gets messed up, while with a 20mm move it doesn't move breaking many features in the timeline. The sketch also references a Pi Boards component edge, with the 10mm change it gets moved to the other side of it, while with the 20mm move it's just completely broken. Looking for some help on what to change to get this sketch to update appropriately when the dimensions are changed.

[jhackney1972]

Please attach your model.

[Anonymous]

Trying again to get the screen cast attached.

Screen Cast

I'm apparently incapable of figuring out how to imbed one.  Hopefully the link works.

[jhackney1972]

The screencast is available and does show the symptoms but I do not think anyone will be able to diagnosis your issue without the actual model file.  Please attach it to your forum question.

[Anonymous]

https://a360.co/2OrUpEL

You can see the screen cast on the original post or through the link in my reply?

[Anonymous]

Played with the model a bit more.  No longer referencing the pi board model at all to place the first post that the board is then jointed to.  Re-added all the projected geometry trying to only pick what was needed and not converting any of it to construction.  Still having the same strange behavior.  Rolling back in the timeline so that only the post and board should move, everything resizes and shifts around nicely changing the length, width and two pi offset values.

Got the middle part moving correctly.  Then I for the first time noticed the very first sketch was getting messed up on resizes.  I deleted a bunch of construction lines and simplified it a bit.  It started with a center rectangle that had fillets applied to it and was converted to entirely construction lines, then had an offset made from it.  I got rid of the crossed construction lines and got the mid point lines that were added for symmetry constraining it to the origin.  Now it doesn't show as fully defined, but I can't get anything to move in the sketch and can't figure out what to add to fully constrain it.  After this the middle part isn't moving correctly anymore.

Any help figuring out what I've done wrong or if this is an actual bug would be greatly appreciated.

[rohit.bapat]

Hello @Anonymous

Sorry to know you are facing this issue and also thank you for reporting it. I have created a ticket FUS-44151 for the development team to take a look at.

Thank you,

Best Regards

Rohit Bapat

[Anonymous]

More playing and I seem to have hit on a combination of constraints that update correctly. Replaced the very detailed pi model with a single solid object that is very simple and oversized slightly so I can use its projected geometry rather than do offsets from it. Then managed to use only two measurements from projected geometry instead of the many I was using before. 

Other odd behavior I was seeing was it not allowing concentric constraints but allowing coincidence on the center point of multiple curves. And not allowing three points to be made horizontal but letting me put a horizontal construction line between them and making that horizontal. 

[jhorstink]

I see this question is not solved yet. Is there some progress?

I have a similar problem, also with a parametrized model. When I change a parameter in the (fully constrained) sketch the bottom line becomes the reference, instead of the upper line.

after changingmodelmodel sketch

[rohit.bapat]

Hello @jhorstink 

We are sorry to hear that you are facing this problem.

But, the good news is that the team has finished working on the ticket FUS-44151 mentioned above. The fix needs to be tested thoroughly before it reaches out to the customers. So the solution should be in Fusion 360 soon. 

Meanwhile, would you be able to send the f3d file which is giving you the issue to my work email rohit.bapat@autodesk.com ? So that we can check if the fix also resolves the problem you are facing. Your data will be kept safe as per our security policy.

Thank you,

Best Regards

Rohit Bapat

(Product Owner)

[Anonymous]

It's a year later and I'm having the same problem. Has this issue been fixed.

[TheCADWhisperer]

File >Export and then Attach your *.f3d file here.

[jhorstink]

Not that I know. After a few weeks animated discussion, silence followed.

[rohit.bapat]

Hello @Anonymous 

We have fixed the original issue FUS-44151 in April 2019 release. Can you please share the f3d file and the steps to reproduce the issue? Maybe it is due to different reasons internally. But, it's difficult to speculate without the file and the steps.

Thank you,

Best Regards

Rohit Bapat

[Anonymous]

I've attach a design and word document, which illustrates the problem.

[g-andresen]

Hi,

I can't reproduce that:

günther

[Anonymous]

Hi Gunther:

I'm confused. The video you show does reproduce the problem. What am I missing.

[jhorstink]

Hi,

When I change the dimension in small steps, the sketch behaves quit normal. Up to 4 when enlarging, 5 or more when making the width smaller. It has something to do with dimension d293: boxsidewallthickness/2, I suppose the sketch 'is not sure' which side this dimension goes when changing the value of BoxLeftToRight.

It often helps when the dimensions come from a stable side, which is not moving when changing the parameters.

Therefore I added a dimension for the groof from the left instead of d293 and then the sketch is stable when enlarging, but unfortunate there are still some troubles when making the width smaller.

Maybe you can solve your problem with this workaround, but it is a flaw in Fusion.

Regards

[Anonymous]

I think we're both on the same page. With only a magnitude dimension with no direction specified there appears to be two valid solutions for the redraw solver to select from. Unfortunately for me, it sometimes picks the wrong one.

I'd obviously like to see Autodesk address this problem. Unfortunately, I'm not sure how.

A possible workaround for me on the boxes I design is to use absolute dimensions from my anchor point, which is the lower left and corner, instead of relative dimensions. Using the symmetry constraint, where I can, would also improve the situation.

[jhorstink]

I agree, dimensioning from the base point will stabilize the sketch.

Even the dimensions from the holes on the right side are not to be trusted (in my sketch d442 and d443). Unfortunately it is complicated to dimension these from the base point, because in a square root Fusion needs dimension-less figures. 

For the time being: use the work-around.

I get the impression not many people are using the parameters, although it is a very, very strong feature of Fusion - when functioning allright.