Sketch Issue - Dimensioning a corner where 3 arcs are tangentially constrained

[ryan]

Any idea why the geometry here becomes over constrained when dimensioning a corner where 3 arcs are tangentially constrained (see attached) The geometry is not actually over constrained, as it can still be manipulated manually by clicking and dragging certain points in the corner most arcs. Additionally, dimensioning does start to work intermittently as the large radius "sides" decrease to under 800-900in. 

I'm sure the math is mind-numbingly complicated but it is math so I'm surprised that it behaves so erratically and actually works under different conditions.  

[jhackney1972]

As I see it, you are missing only one dimension to make to sketch fully constrained.

[ryan]

Sorry maybe I was unclear, the goal isn't to fully constrain the sketch. The goal is to create parameters that control the the x and y distance of the corner(2in)-arc-centerpoint to the origin of the model. However, the sketch will not accept this kind of linear dimension, it gives me an error message saying that the sketch is over constrained...even though the lines are still "blue."

I have tried the other route as you have shown, by dimensioning the radius rather than the linear position and it works UNTIL you exeeded values above 1000in for the the side and end arc radius(ie. as you approach a rectangular shape with r2in corners) As the side arcs approach straight lines the model won't accept the values (>1000in) and the tangent constraints in the sketch show up red (err).

[ryan]

My first thought is that there may be some kind of limit or singularity event in the programming math of the fusion modeling engine as the larger arcs in tangent constraints approach x=0 or y=0, in other words some value is approaching ∞ or 0 and won’t compute. I just thought I'd have to be a lot closer to a straight line to hit that kind of limit.

I can potentially remove the corner radius from the sketch and add it in later as a fillet but I’d like to keep it in the sketch if possible, as that workaround introduces other programming complications later on.

[davebYYPCU]

Keeping sketches simple is often all that fixes these things.  Your parameter dimensions.

May not suit your purposes but mirror the plate x 2 may work.

Might help...

[ryan]

Thanks @davebYYPCU I have in fact tried this method to no avail. Mirroring has worked well for me in other complex sketch scenarios but not in this one unfortunately...at least for the parameter values I am try to pass to the sketch. See below...arc height values above 1" seem to work fine but below that, its unreliable. 

Interestingly, I can get down to about a 0.1" arc height, but I have to enter a series of 3-4 decremental values starting above 1" (ie 1", 0.5", 0.25", 0.1") the model will not go from a value of 4" to .01" directly. It's like I'm asking it to polar bear swim but it will only do it if it can wade in a little at a time. 🤔

 

 

[ryan]

Here's is a more isolated example of the problem I am having. Everything seems to work until I start entering a range of parameter values, especially going from small (<0.1") to larger values (4-20") and back.

 

[davebYYPCU]

My testing of my sketch did not break, 3 tangent curves, doing one instead of 4 off, gives Fusion a fighting chance.
Not talking about Sketch Mirror.

There are no fillets now, should be even simpler.
So you are dimensioning an arc with arc height?

What range of parameters are involved?

Sorry didn’t know you were responding.

I found your original sketch corrupted, is this one also corrupted?
Have you tried Compute All?

[ryan]

I know you weren't talking about mirrors as a solution, it just necessitates mirrors to achieve a closed shape. Even simplifying to just 2 arcs + mirrors (in my 2nd example) or to a single arc (my 3rd example) it still breaks when the radius exceeds 1000" or arc height <.1"

I did try compute all and it didn't resolve anything.

I'm not sure if the latest model I posted with just the pinned arc has a corrupt sketch, I would think it might be as well given that I have broken it to show the errors. 

I don't really care how I have to dimension the sketch (corner point xy vs arc height vs. arc radius) they all exhibit the same issue of not handling the toggling of parameter control values such that the arc goes from almost a straight line to a distinct curve and back. 

[davebYYPCU · Accepted solution]

Huge relative parameter value changes have been a problem for a long time, incremental steps as a work around has been the Autodesk solution.

Might help…..

[ryan]

Ahhhhh...I did not know that. That is helpful information. So basically if I want this exactly method to function seamlessly I would have to write some kind of script that loops incrementing/decrementing parameter values on an exponential curve based on my expected  range...sigh. Too bad it wasn't an easy bug fix