Parametric model breaks when changing parameters by larger values but works fine when performing the changes in smaller increments

[josephNWHGZ]

Hello, I am trying to design a parametric range hood model that I can use as a starting point for custom designs. Ideally I want it to encapsulate all the sheet metal parts and include some of the basic templates used to make them. 

When I first started this seemed like it would be fairly straight forward to make something like this but every time I am 90% of the way there something breaks in some strange way. Currently when I try to change parameters it works great sometimes and not at all others. 

For example, if you were to change the upper flange length from 45" to 15" it would work fine but if you try to change from 45" to 5" it breaks irreparably. What is really strange is that if you change from 45" to 15" then from 15" to 5" it works fine? The sketches appear to be fully constrained and I cannot find anywhere to add further constraints.

What am I missing or doing wrong?

Also I can create python scripts to assist with this process if necessary.

[johnsonshiue]

Hi! This is a sketch solving inconsistent issue. It could be related to the tangent constraints between the arcs, particularly small ones. I would delete the round corners of 0.125 from sketches. Then create Fillets on those sharp edges instead.

Many thanks!

[laughingcreek · Accepted solution]

sometimes certain arrangements of dims and constraints will trip the sketch solver up, particularly when making large value changes.  you can usually over come it by trying to constrain in a different way.  here are a few things I would suggest to make this more stable-

-use projections.  you use upper flange length in all of your sketches.  instead use it just once in the first sketch, then project the end points of the line it controls into the other 2 sketches and coincident to the projections.  (incidentally,  the first sketch doesn't fail when changing upper flange, so this one change is all you need to do to fix the model.)

-simplify the sketches by not putting the thickness in the sketch. do that in the solid space.

-take advantage of symmetry.  the hood is symmetric left to right, so center it on the origin plane.

-related to above, you only have to model one side. the other side can be mirrored.

-it's not necessarily wrong to put fillet arcs in sketches, but can be easier to control things if you apply the fillet in the model space instead.

attached is a workflow that uses all of the above

[davebYYPCU]

Ideally, I want it to encapsulate all the sheet metal parts and include some of the basic templates used to make them. 

Not a bad idea.

.... What am I missing or doing wrong?

You are working too hard and those bodies are not going to convert to Sheet Metal (tried it?)

The chain of tangent curves will always solve in short increments, you will have to work around that, changing values incrementally to get to the range of allowable.

To get Sheetmetal compatible parts for these sketches, you will need extrude / cut etc as surface bodies and then Thicken.  Therefore, the offset thickness in these sketches are not necessary.  Could be construction for prompting a few years later.

(Too slow .. yeah what Alex said)

Might help....

[josephNWHGZ]

Very helpful reply! Trying to include the radius in the sketches was probably my biggest problem. Using the fillet command in the timeline instead fixed pretty much all my issues. Projecting from sketch 1 to sketch 2 and centering the hood at the origin are also good suggestions as they help simplify the model and make it easier to work with once you get into unfolding the sheet metal and making the templates.