Can't complete constraints and showing constrained when it isn't

[douglas.angle2]

Relatively new user, and I don't really understand the constraint system well enough.  There are a couple of problems with my sketch:

- an arc is showing fully constrained, but the end of the arc does not touch the object it should be coincident with (there's a small gap circled in the image below), and there's no constraint showing on the end of the arc that would limit it.  I can't extend the arc until it touches or add a coincident constraint.  What's making it fully constrained? How do I fix it?  I also need some help with the corresponding arc on the opposite side - why isn't it fully constrained?

- There is an arc, line and spline that appear to be fully constrained but not showing as such.  I can't move any of the vertices, so the constraints must be there but they show as blue, not black.  Attempts to add further constraints either just don't work, give an "over constrained" error or give a "cannot compute" warning.

While we're at it, how can I tell what objects a constraint marker is referring to?

[TheCADWhisperer]

Click and drag the white dots.

What do you observe?

Are you familiar with the Coincident Constraint?

[TheCADWhisperer]

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@douglas.angle2 wrote:

I also need some help with the corresponding arc on the opposite side - why isn't it fully constrained?

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Is it Tangent Constrained to the Ø7 circle?  (Tip: Answer is no.)

When you finish this design - I recommend that you Attach it here for diagnosis by the experts.

I suspect that they will demonstrate that you are working too hard.

Is this part the same one you posted about before - or is this a mating part to that part?

Is your Origin Center Point at a logical location in the sketch?

Are all dimensions measurable with standard measuring instruments?

Could any of the arcs be added as placed Fillet Features rather than as sketch elements?

Is there a logical reason that you used a Spline rather than an arc on the right side of the sketch?  (And what cutting tool will be used to create that feature in the real world?)

[TheCADWhisperer]

Most Fillets should be Placed Features (not sketch elements).

[douglas.angle2]

When I try to click and drag the white dots don't move.
Coincident constraint did nothing, and didn't give an error or warning.

[douglas.angle2]

> Is it Tangent Constrained to the Ø7 circle? (Tip: Answer is no.)
No, it should be coincident constrained instead.

> When you finish this design - I recommend that you Attach it here for diagnosis by the experts.
Ok.

> I suspect that they will demonstrate that you are working too hard.
Hence the post!

> Is this part the same one you posted about before - or is this a mating part to that part?
I had posted a mostly complete design with some issues of fillets and draft. Advice there was to go back to a fully constrained sketch. This post is the first of the required sketches. There is no mating part, although this box also holds an arm with another bearing block on it (but all one piece).

> Is your Origin Center Point at a logical location in the sketch?
I don't understand the question. Why does it matter? If anything, the origin is in the center.

> Are all dimensions measurable with standard measuring instruments?
Do you mean in fusion or in real life? I have measurements for the linear dimensions, but not the radii of the arcs.

> Could any of the arcs be added as placed Fillet Features rather than as sketch elements?
Some, but they aren't necessarily fillets, ie may not be constant radius and/or tangent/perpendicular.

> Is there a logical reason that you used a Spline rather than an arc on the right side of the sketch?
That's the shape of the origianl.

> (And what cutting tool will be used to create that feature in the real world?)
The part is a casting; the pattern would have been made from maple. The curves could well have been cut by hand with a drawknife.

[douglas.angle2]

> Most Fillets should be Placed Features (not sketch elements).

By "placed feature" do you mean using the fillet function after the part is extruded? 

If so, how would I use that in place of a spline, or when the arc isn't tangent at the ends as in a fillet?

Here's the part I'm trying to model (note drawing is a mirror image of the photo):

Thank you for taking the time to reply.

[TheCADWhisperer]

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@douglas.angle2 wrote:
When I try to click and drag the white dots don't move.

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That's interesting.  

There must be something wrong with your install of  Fusion 360 as I can easily drag them (video to follow in a few minutes)...

[TheCADWhisperer · Accepted solution]

@douglas.angle2 

[douglas.angle2]

Thanks for the video.  That was great!

As for weird dimensions like 1.50007, those were all typed as round numbers when the feature was created.  Then when I dimensioned them, the extra decimals showed up.  Somehow Fusion adjusted the dimensions by a small amount after they were entered.  Perhaps some tiny movement when features were constrained?

i see that I missed a number of coincident constraints.  This was something that I'm confused about (see the title for example).  Why does the line/arc/etc show black as if fully constrained when it in fact the endpoint isn't constrained?

You may have a valid concern about reducing complexity for cost of manufacture in general.  In this case, it's going to be 3D printed to be used as a pattern for sand casting (in 1/8th scale).  Complexity isn't an issue.  Now granted, the spline is only cosmetic and has no particular function above what a fillet would, but it would be nice to have it as close as possible to the original shape. 

Anyway awesome video.  It was well done and cleared up a number of things.  Still can't constrain the blue lines on the right side though :(.

[jeffescott]

The spline handles are not constrained.   Each one needs a length and angle and each point needs to be constrained

[jeffescott]

4 constraints per point. Xy of point. Length of handle angle of handle.

Or xy point xy of one handle end

[douglas.angle2]

For the spline:
Bottom point: xy of point is coincident constrained by the length of the line. As a check, I can't move that point.
Length of handle is dimensioned. Angle is defined by the tangent constraint.
Upper point handle is constrained by xy dimensions.
Point is constrained to the corner(?). There's a coincident constraint there, but I'm unclear if that's the two lines or the spline and the line. Either way, if I attempt to add the constraint there, I get an "overconstrained" error.
I get what you're saying, but I'm not clear how to interpret in in this sketch. Which of the 4 constraints am I missing and on which end?

Any thoughts on the fillet and the vertical line? Why are they still showing blue? Again, any constraint I try to add gives me an error.

[jeffescott]

I refer to you second sketch in the first post. The “handles” are blue. They are not constrained. Try moving one end of the handle either up or down or longer shorter it will move. The spline will change shape. Each point along the spline has a handle. Each handle must be constrained. You can select fix and fix each point where it is. Not really elegant though.

The handles can be tough to see if nearly parallel to the spline

Create mew sketch then a spline with three points. You will need 12 constraints to fully constrain

[jeffescott]

The handle which you constraint with a single dimension 1.05 does not fully constraint that point.   Try moving that point up and down

[douglas.angle2]

Ok, I finally got it.
Deleted the vertical line so I could focus on the spline. I discovered that a dimension from end point to end point fully constrained the spline. So the endpoints weren't constrained as much as I thought. Then added the vertical line back, and with some more constraint, got the whole thing done.

> The handle which you constraint with a single dimension 1.05 does not fully constraint that point. Try moving that point up and down

It appears this wasn't quite it. The 1.05 defined the length of the handle and the tangent constraint defined the angle so the handle was in fact fully constrained to the endpoint. I couldn't move those handles up and down. (as zero degrees) But defining the length of the spline as described above fixed the endpoints. Then the 1.05 dimension is from a fixed point at a fixed angle so it became constrained as well.

Thanks jscott65WZG and CadWhisperer for your help. And I promise to fix the weird 6 decimal place dimensions too!

[etfrench · Accepted solution]

End points may not be fully constrained even if the line/curve/spline is shown as fully constrained.  We have yet to convince Autodesk this is a bug😊

[douglas.angle2]

Thank you for the confirmation on that. Hello Autodesk - it's a bug.

[TheCADWhisperer]

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@douglas.angle2 wrote:
And I promise to fix the weird 6 decimal place dimensions too!

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@douglas.angle2 

I’m still curious how those are occurring in the first place?

[jeffescott]

the error appears to be in the solver.   If the constraints provide no solution but allow the solution to begin to converge on an answer. Then if the solution is within the set tolerance of the solver it provides that as an answer.  Results in closed solution indicated but not precise.   

click accept solution and pose another question