sketch parameters/constraints going haywire

[Anonymous]

I have tried several times now to create a fully parameterized version of this sketch. It's a portion of a case for cell phones and my intent is to make the sketch easy to adjust to various cell phone dimensions (in particular height, width and corner radiuses). Everything I have done up to this point has failed.

For the larger rectangle with filleted corners I defined the height, width and fillet radius:

Radius = 10 (and I set all 8 of the fillets equal to it)

LHeight = 172 (and I set all 4 vertical edges equal to it)

LWidth = 86 (and I set all 4 horizontal edges equal to this one)

For the narrower rectangular sections I defined the height and width:

NHeight = LHeight - 2*Radius (I want the smaller, narrower rectangles to always remain vertical centered and adjust their heights accordingly)

NWidth = 12

Inset = Radius (inset is the vertical alignment of those narrower rectangles. I purposely want the inset to be exactly equally to the fillet radius)

But the moment I change Radius larger or smaller, the entire sketch gets screwed up. I'm talking completely haywire.  The sketch becomes distorted/skewed/tangled/etc. So I began setting sketch constraints in various combinations of perpendicular, parallel, collinear, equal, etc to force the edges to remain appropriately parallel and perpendicular, no matter what value I set for the fillet radius.

None of it has worked and I suspect I am overlooking something very simple here.  If anyone might have some idea how to constrain this sketch so that I may set LHeight, LWidth, NWidth and Radius, I'd appreciate the insight. Or if you suspect I missed something with the current sketch, I could really use the insight.

Cheers,

Joe

[Anonymous]

I should mention that the sketch in the screenshot is not the sketch I had been working with all along. I just quickly threw together the same dimensions using 4 separate rectangles so I could give you an idea of the shape I've been trying to create. The actual sketch would consist of just one piece as shown in this diagram, attached.

[daniel_lyall]

Can you post your file it will be a constraint or diamention placement doing it Go to File -> Export and save as a .F3D Archive File and attach it to your next post.

[Anonymous]

Hi Daniel,  

Sure, this is just one of many attempts. In this attempt I ended up with an overconstrained sketch.

So that you can see what happens, I left several fillets off of this sketch. Try adding new fillets to the edges of the largest rectangles. Use the defined Radius parameter and watch what happens to the sketch. I have attached a screenshot that shows how the addition of one fillet skewed the entire sketch.

Cheers,

Joe

[daniel_lyall · Accepted solution]

So far the sketch is way over constrained thats why it was going up on a angle, I removed all the fillets, constraints and dimensions then replaced all the dimensions then applied a few constraints to make sure everything stays in line when a change gets done, then tested it to death to make sure it does not break.

Now to adding fillets in the sketch it is not a recommended thing to do as if a constraint or diamention is not in the correct spot it will break even if it was fine before the fillets got added you could say you need to be aware of this before doing it.

What is recommended is to put the fillets in on the solid right at the end, it's up to you how you do it now as you have been informed.

Attached is your file with no fillets but it is stable. now are you able to apply the fillets in the solid not the sketch it's your design intent 

[davebYYPCU]

One more constraint, 

make the vertical line above the Origin Vertically constrained.

Change of radius doesn't break it if you do that. (tested with 8mm & 12mm)

I was under the impression that until the sketch is fully constrained, (weird) unexpected things can happen, might be wrong.

Might help....

[daniel_lyall]

It depends on the dimensions if they are in the correct spot and linked it might not break.

[davebYYPCU]

Sketch was able to rotate on the Origin without breaking anything else, 

was not fully constrained when it arrived, 

Joe wants to drive the sketch with radius changes, 

stop the rotation, all good?

[daniel_lyall · Accepted solution]

There are different ways to do it, it's up to joe how he does it, I just like to reduces the overhead on sketch's.

Just a test I am not arguing or anything just seeing if someone else hits the bug I have found, put the constraint in as you say to do then match the fillet up the top like it is on the bottom on the right side and see if the diamention d16 inset goes banana's. 

[davebYYPCU]

Ok, something astray now, radius restored to 10 and red constraint errors.Will go back.

[davebYYPCU]

Working now, don't know what I did to break and fix it, without doing anything but edit the radius parameter.

My version didn't have a top right radius.

Will see what Joe says....

[Anonymous]

Good morning Dave and Daniel,

First, thank you both for taking time out of your day to try to help me with this funky issue.

I did begin with no constraints at all. When I found that the sketch breaks due to adding fillets, I began adding constraints.  First just a couple to keep things perpendicular, or parallel or vertical, etc. When none of my combinations worked I got more aggressive with the constraints to the point that Fusion warned that the sketch was over-constrained. Here's the takeaway from my experiment...no matter how much or how little we constrain this model, it breaks with the introduction of fillets.

Crazier still, the fillet that breaks the sketch will not necessarily be the same one each time. There are times when I would successfully add 3 or 4, and the 5th would break it. Sometimes the 1st would do it and other times I'd make it all the way to the 8th and break it. There are times when one on the left, or right or in the center breaks the sketch.  There's no rhyme or reason to it. But wait, there's more. The type of distortion isn't consistent. The addition of a fillet at a particular location in the sketch can break that sketch in different ways each time that you apply it. Apply it the first time, and maybe the sketch ends up slightly rotated or skewed. Undo it and apply it again and this time maybe the inset becomes half the fillet radius despite being a user parameter equal to the fillet radius.

In the attached image, I played with the new file that both of you took the time to rework and test (which I appreciated very much, thank you both). I began by simply adding fillets from the top left corner, working my way to the right. My results:

• A shows the successful addition of the 1st fillet. 
• B shows the successful addition of the 2nd fillet. So far so good.
• C shows how the 3rd broke the sketch in a very specific way...Inset is now incorrect and its dimension lines are angled. When this happened I undid the change back to the second fillet and began adding again. Magically, I was able to add a 3rd fillet this time with no issue.
• D shows how the addition of the 4th fillet broke the 2nd and 3rd fillets in quite an unusual way.

So even this newer vetted sketch is not able to handle the addition of all 8 fillets without breaking. Structurally, if the inset (as I've defined it) is equal to the fillet radius then none of this should happen. Fusion appears not to handle fillets very well when they're in close proximity to inside corners. Or perhaps when their are so many on a single sketch. 

Perhaps I could create this sketch as 4 independent rectangles, two larger with all 4 corners filleted, and two smaller/narrower. But I'm not familiar enough with Fusion to know if this will create other issues for me downstream.

Daniel, something you had written raised another question for me. You suggested that I add the fillets later on the model, not on the sketch. I assume I'd tie those fillet parameters back into the ones used by the sketch rather than placing the burden of all the parameters on a single sketch. I'll try toying around with this. I had not thought of it. I became obsessed with figuring out why fillets that should work, would not, when I really just need to get this done to move on to the other components.

Thank you both again. I truly appreciated the help.

Cheers,

Joe

[Anonymous]

Voila! Daniel, thank you for your advice about simply using fewer parameters on the sketch. That worked beautifully. 

My original mindset was to place all the parameters on the sketch. That failed repeatedly. By moving just the fillet parameter off to the body -- problem solved! I now have all the customization I hoped to get with none of the issues. Of course I wish it had worked on the sketch, but this works beautifully.  Onward and upward!

Thank you, thank you!

[daniel_lyall]

 I got it working and updating very nicely, there was two things manly doing it.

Having the dimensions on the points on the outside plus the missing constraint dave said to add in.

This was why the model popped up on a angle as the fillets had nowhere to go, you increase the size with the width not fully constrained it will just go bananana, the length was the same it did not know to just go wider and higher.

Too many constraints plus the wrong type.

Some of the constraints were doing the same thing.

That's why I said right from the start it will be a diamention or constraint doing it been there done that, 9 times out of 10 everyone comes across this problem.

I have attached my version so you can just look over it and see what I did, it's my way of doing it (is the best way to put it) this is one of the good things about this forum you will be given examples sometimes many and you can do what you wont with it, we are here to help not say do this or that or piss off.

I also added a width diamention in it to show how to lock the width down without breaking it.

[davebYYPCU]

Haven't checked Dan's new file, was working on my brain teaser.

I would like to know if it can be broken.

Basically you have vertical symmetry and a horizontal duplicate.

I believe that adding fillets was causing the trouble, over doing circles first and trimming them with external lines 

Might help

[daniel_lyall]

Thats a interesting way to do it that works very well

[Anonymous]

I figured eventually I went overboard with the constraints...down a dead end road. It got to a point that I finally caved and wrote in to the forum for help. 

[TrippyLighting]

I could not help myself. I always like a good sketch challenge. The challenge for me usually boils down how to sketch as little as possible 😉

2 Center rectangles. 2 Lines to connect the 2 + 3 lines for the tab on the right. Fillets are on the solid (of course).

Model is attached.

[Anonymous]

I'll keep that alternative method in mind if I run into this again in the future, Dave, thanks.

This case design consists of several components, each dependent on the main component generated from that sketch.  So figuring out that sketch finally put the last piece of the puzzle in place. Rather than having to recreate the case from scratch for each unique cellphone length, width, corner radius and thickness, I can now change fewer than a half dozen values and the entire design...every component...resizes to fit another phone. 

I'm not new to 3D modeling. I spent about a 15 years using all sorts of modeling apps, from AutoCAD and the more unusual TruSpace, to SW, LW, Povray and Hash Animation. But I haven't touched CAD in at least a decade since then.  I picked up Fusion last week and all I can say is WOW! I'm not sure which I love more....the app which has been a breeze to learn, or the awesome community of Fusion users that have come together to support each other.

Thanks guys!

[Anonymous]

Now that is another creative approach that never dawned on me. Thanks for the added inspiration Peter.