Degrees of freedom: how to find remaining.

[JJHawg]

I have been drawing my 2D sketches very carefully, trying to minimize DOF while drawing. However, I can't avoid finishing a sketch and still have some open items. I can use "Analyze" to sometimes find problems, but after that I end up trying to drag sketch elements around to see what moves. Unfortunately, frequently nothing will move, even though officially the sketch is not fully constrained.

So, the question is, are there any tips or tricks to finding these remaining DOF items?

Also, I sometimes feel that the automatic drawing constraints feature gets in my way, does anyone else feel this way?

Note: I am having strange results when trying to fillet an extrusion that was created with a DOF = 1 sketch, and I suspect that this is the source of the problem...

Thanks,
Jim

 

[MilesH]

Jim,

Auto-Dimension can be useful for tracking down the remaining DOFs - you can Undo if you don't like the way it does it

Holding down Control + Shift keys overrides Auto-Constraints while sketching.

 

[JJHawg]

Thanks, Miles, for the quick and informative reply.

The auto-dimension trick does help find things left to constrain, but it didn't solve my main problem...

I am making a fairly simple part, one extrusion, one cut, and some fillets. When I try to apply the 3D fillets, some of the curved edges fly off into space, and I get complex geometry errors.

One thing that may be related is the complaint about the first extrusion that I can't figure out. Like I said, this is a simple part, and I think I have constrained everything properly.

I have attached a file in case you, or anyone else, has time to take a look at it...

Thanks,
Jim

 

[DavidJ]

The face selected for the failed fillet does indeed show up a strange extra edge in free space. I can't immediately see why.

 

[DavidJ]

OK - sorted it. The problem is where the face selected startes to curl up over the 'hook'.

Instead of applying the fillet to the face - select all the external edges PLUS the two edges of the curve from the original face into the 'hook' (just the first short curved edges is enough, but you can go as far as you want).

[EDIT - forgot to mention, you should probably uncheck 'tangent propagate' or you won't be able to select the edges individually - in which case I think the problem may come back again]

 

[JJHawg]

Thanks for the information, David.

I like the convenience of selecting faces instead of individual edges, but since technically the fillet is being applied to the "edge", I can do it that way.

However, even when selecting edges, I get the off-in-space fillet at the rounded end of the part. In the file I sent, Edges 49 and 50 both exhibit this behavior, as well as others...

I have never had this problem with round holes, just the obround and rounded ends. I used to make the obround holes manually with two holes and tangent lines, but was a good-boy on this one and use the built-in obround feature.

I may try constructing these features without using the tangent sketch constraint and see if I get different results. Another test is to make the radius of the end section slightly larger than the width of the part, and see if the precise alignment of the various lines is a problem.

Thanks,
Jim

 

[DavidJ]

I think (but haven't explored fully) that the problem is related to the bend in the part. If you select the face, you are including a boundary where physically it's impossible for the fillet to go in the same direction as on all the edges - hence confusion.

In most cases you can happily select a face and hence fillet all edges in one go - but if the fillet has to change from convex to concave in the process there will be an error.

Did you make turn off 'tangent propagate' so that you can select each edge section individually - by adding one at a time, you should see where the issue is?

 

[denisgb2]

Jim,

I am using 11.1 and I opened your part. As soon as I went in and out of edit for sketch 1 I received an extrusion error. I deleted the extrusion and then received a sketch error. I next created a new part and copied the sketch from your part to the new part, the copy sketch stripped many constraints and dimensions, auto dimensioned the sketch, redid the extrusion, and had no further errors. Copied the extrude cut, fillet 3, and fillet 4, and fillet 4 failed as per your model. Tangent propogate made no difference, selected of not.

As David pointed out, it seems that the face fillet in question will fail unless you also select the adjoininig inside curved face. I added the adjoining face to fillet 4 and regenerated the part with no errors.

I went back to your part, edited fillet 4 and added face #19 and the model regenerated the fillet with no errors. However the Extrusion 1 error mentioned above persisted. I am guessing there are conflicts with the multiple sketch constraints, some of which were dropped when I copied your sketch for my model.

Interesting.