Underconstrained sketch, but any additional constraints are "overconstraining"

[grzesiek.wilczek]

Hi everyone.

Can someone explain to me, how do constrains ACTUALLY work?

How is that even possible to have a square with ONE unconstrained edge? Which cannot be moved or modified in any way? Why is it unconstrained then? Attempts of adding any sort of constaint to it results in "sketch overconstrained" error?

The octagonal shapes are even more confusing - I can actually move some of the unconstrained vertical lines to the left or right, but if I try to constrain them by specifying a distance from another line I get overconstraied error again! Even though I physically can change the distance I have in mind by dragging the line (right vertical edge of the first octagonal hole from the right)...

I know, I am using a lot of "equals" constraints, so maybe there's a way of limiting the usage of them, if I want to repeat identical cuts across a solid?

Problematic design here

[jeff_strater]

you have not marked this link to "allow download"

[grzesiek.wilczek]

I can't do it - it's a paid feature. Can I share it any other way?

[jeff_strater]

ah, OK, then the next best approach is to Export this as a Fusion archive:

This will export the design to your local drive.  Attach it to your forum response.

[grzesiek.wilczek]

Thanks, there it goes:

[jeff_strater]

it wasn't completely clear which rectangle you were talking about.  I found a couple which were legitimately underconstrained, bad one which appears to be incorrectly colored.  That one seems like a bug to me

Your theories around Equal constraints are probably correct.  I noticed if I removed one Equal constraint, and replaced it with a dimension (didn't even need a second dimension), these rectangles showed fully constrained:

Personally, I stay away from Equal, not for any good reason, simply because I prefer dimensions, and setting values to be equal as a way to enforce that length equality.  But, your sketch should be valid, as well.

[grzesiek.wilczek]

First of all, thanks for your time & effort to investigate. I really appreciate that.

If you take a look at far right, there are three octagonal slots, and they are also not fully constrained, though not editable either.

Anyway, I'm "glad" to hear that the bottom right square from the screenshot is actually a bug, not my ignorance 🙂

Do you have any hints on reptetive slots like in my sketch? I'm not really happy with the idea of typing dimensions for every single one of them, especially as it might be required to alter them at later stage. So I assumed I'd create one and then just make all others equal and co-linear where possible to create a grid. Clearly this is not the cleanest solution, so I'm open for any hints & tips.

[TheCADWhisperer]

This doesn't directly address your issue, but if it were my design I would -

Break up the sketch into at least two sketches.

Add Chamfers (or Fillets) as Placed Features rather than Sketch elements (if possible and practical).

And I generally do not repeat dimensions. (Unlike @jeff_strater , I prefer = rather than repeated dimensions.)

I found it painful how many repeated dimensions you have.

Edit:  I would expect to start seeing issues with a sketch like this.

[grzesiek.wilczek]

Thanks, I'll explore that, although I do need it for laser cutting, so I though I'd need everything on the sketch to export the sketch as DXF. Can I export a face created the way you described into DXF?

[TheCADWhisperer]

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@grzesiek.wilczek wrote:

 Can I export a face created the way you described into DXF?

---

Yes.

This would be my Sketch1.

Edit:  Change that 96 to 104.  Back in a few minutes with revised example...

See Attached...

[davebYYPCU]

Yes, you need an Addin from Github, called DXFer.

select any / all faces of a model, for output into one dxf file.

This workflow is before the new nesting functions in Fusion, but I have a good system going with DXFer.

in your case sketch one each Extrude Cut Profile, Pattern the extruded Cuts, and extract the body face.

Might help....

[TheCADWhisperer]

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@davebYYPCU wrote:

Yes, you need an Addin from Github, called DXFer.

I just did it without any add-ins.

[davebYYPCU]

I'll choice my words more wisely, (scratch the word need)

Laser cutters rarely have just one part in a file, DXFer outputs multiple faces into one file, without duplicating sketches to get there, where as Fusions native, Save as DXF outputs one sketch to one file. 

May well be redundant now that Nesting has been rolled out.

[grzesiek.wilczek]

My cutting provider requests  each part as a separate DXF (online pricing), but I'll definitely give it a shot.

[JamieGilchrist]

HI @grzesiek.wilczek,

everybody's advice in here is on point.  I'll just add for emphasis, always try to distill you sketches to the bare minimum of information to create your geometry, and progressively add more detail and try to use modeling features for details over sketches whenever possible.  I took an approach similar to @TheCADWhisperers:

Sketch:

 

Extruded body:

 

Chamfers:

Pattern 1:

Pattern 2:

...

Patterns 3 & 4:

Created a new sketch (offset plane just for clearer illustration) and projected the top face:

now your model is the source of truth and any subsequent data for export verification, etc. is driven from that source.

hope this helps

 

 

 

 

 

 

[davebYYPCU]

Thanks Jamie, nicely illustrating my point, 

Your last step, projecting the body into a duplicated sketch, is not required when using DXFer, selecting the face, exports directly to dxf.

Might help....