Why Can't I Fully Constrain this Sketch?

[Anonymous]

The following sketch is being copied from a paper print.  I cannot figure out why it will not fully constrain.  A few hypotheses:

-Perhaps it has something to do with the fillets.  The fillets are not specifically defined on the drawing.  I chose a fillet that looks like the profile in the drawing. 

-Perhaps it has something to do with decimals being rounded to .001".  For example, 5/32 = 0.15625, but Fusion rounds this to 0.156.

Notes: I believe I attached the file correctly.  If I need to do something else to share it, please let me know what steps to take.

Also, I made the holes .063 to allow for reaming as called for in the drawing.

Thanks,

Marty

[HughesTooling]

Your horizontal centre line is not constrained. You have some overlapping points that make it hard to see what's constrained. Just try dragging the circle.

Mark

[MRWakefield]

@HughesToolingjust beat me to it! Take a look at the attached screencast which shows how to fully constrain your sketch with one additional coincident constraint.

Edit: Ok, so the forum is still playing up as regards embedding screencasts! I'll be back soon with the screencast...

Ok, try this: https://autode.sk/3bvq13P

[HughesTooling]

You also have something wonky at the other end with the 0.125 dimension. You can see the dimension lines are at a slight angle. You can fix it by deleting the dimension and constraints then reply but I'd recommend you keep the sketch simple and add the fillets to the model and keep sharp corners in the sketch. Best practice is keep your sketches as simple as possible and use solid fillets, chamfer etc. if practical.

Mark

[Anonymous]

Ok.  I can see the problems with the single-hole end of the piece.  Are you saying to leave off the fillets for now and add when I extrude the piece to final thickness?  That way I am working from a fully constrained sketch.

Also, the long sides are supposed to have a slight taper to them.

Thanks,

Marty

[Anonymous]

How do you suggest I constrain the horizontal construction line?  I thought I had done that. 

[TheCADWhisperer]

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@Anonymous wrote:

-Perhaps it has something to do with decimals being rounded to .001".  For example, 5/32 = 0.15625, but Fusion rounds this to 0.156.

Also, I made the holes .063 to allow for reaming as called for in the drawing.

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Examine the Attached file.

Note the simplicity of the sketch.

Use Equal (=) constraints where appropriate.

Not sure what you 1 inch offset was for, but in general you should not have any dimensions on your sketch that were not on the original drawing.

Double click on my 1.781 dimension.

Note that it was entered as a formula.

Even if dimensions are only displayed to three decimal places - in the background Fusion calculates to I think 15 or 16 decimal places.  (Eight for sure.)

And as noted by others - add Fillets as placed features rather than sketch elements when possible and practical.

[Anonymous]

@MRWakefield@HughesTooling Thank you both for your help.  The problem with the sketch was the lack of hole concentricity.  It was a simple fix.  I'm learning more every day I use the program. 

Marty