Sketch is fully constrained but not defined

[mowen34]

I have attempted to add additional constraints to every edge and vertex present however any additional constraint is met with 'Sketch geometry is over constrained.' In addition I have attempted to follow multiple youtube tutorials to no avail.

The text command 'Sketch.ShowUnderconstrained' returns:

'Under constrained points: 16, under constrained curves: 8'

The only fix that has worked is using the Fix/Unfix command on any line segment however that feels like the improper way to resolve this issue.

Any help and/or tips to avoid this situation in the future is greatly appreciated!

[TheCADWhisperer]

• @mowen34 

Missing constraints.
Can you File>Export your *.f3d file to your local drive and then Attach it here to a Reply?

Construction lines.

Colinear constraint.

Tangents

Equal

No need to duplicate dimensions. 

[SaeedHamza]

Here is one way to do it, and please note that this is a case where you're using the origin point to constrain your sketch, and if you don't wanna use it, you can always create lines/points that are fixed (fixed constraint) to be the reference for your dimensions.

[etfrench]

The key in this sketch is to constrain as you go. 

Dimension and constrain the first three lines and add a centerline for mirroring.

Offset the three lines and add the end line:

And finally mirror them:

[TheCADWhisperer]

@mowen34 

Where did you go?

We can cover this step-by-step, but you will need to contribute to the discussion.

I generally avoid Symmetry constraint (or Mirror) in sketch as it is a form of a sketch pattern.

See Attached file.

In fact, with Thin Feature the sketch can be simplified even further...

[mowen34]

Apologies, I posted this, decided to finish the model without everything completely locked down, and went to bed.

Attached you will find the f3d file of the model. Stetch4 is the one in question and sketch7 is using the same technique that caused this issue. From your response, and the other responses I've seen, it seems that there are only a couple techniques that work well, and they're rather unintuitive for a new user. (I'm moving over from C4D, which I primarily use for interior modeling and 3D printing) Is there a written guide on best practices you can link me to?

I'm also aware of another weird bug that I didn't catch as I was moving quickly last night, most of the extrusion for sketch7 somehow folded itself into the body from the extrusion of sketch4 while a small portion was given its own body. Is there an easy way to correct this?

P.S. Feel free to roast any other bad design choices I made lol.

[TheCADWhisperer]

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@mowen34 wrote:

Stetch4 is the one in question 

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Sketch4 is a 3D sketch.

Research the BORN Technique... ...works in ANY CAD software.

@mowen34 

Better to use Full Round Fillets rather than Edge Fillets for something like this - will automatically update if the Extrusion thickness is changed...

Edit Sketch7

Click and drag line and line endpoints.  What do you observe?

Why are there 3 lines here when one line would suffice?

Why, oh why is a rectangular peg used to create a cylinder?

Add a Centerline to the rectangle and Revolve instead...

Or Origin is not in an optimal location.

Model with Symmetry about the Origin will save lots of work.

We cannot manufacture perfect parts - design in appropriate clearance between mating parts.

Is Body3 correct?

I would expect this to be multiple bodies (and eventually converted to Components with Joints for motion on DoF).

@mowen34 

How interested are you in learning to do all of this correctly? (Warning - will require starting over from scratch, my way or the highway as they say.)

[laughingcreek]

sketch4 has been "moved" off the sketch plane, effectively making it a 3d sketch as far as fusion is concerned.  Not a good idea.

[mowen34]

I'm definitely interested in learning to do it right. I've always found starting with a naive implementation of what I want to do and iterating to a correct version is much more conducive to learning what I actually need as opposed to watching/duplicating dozens of tutorials and then still running into issues when I design what I need. (Which isn't to say I haven't watched a number of tutorials already)

Allow me to add some context to the project. The 3-axis gimbal will be mounted underneath a custom drone.  I've already made a rough model of the drone in C4D and I am attempting to transition the design into Fusion so I can accurately 3D print components for prototyping and eventually create molds for forged carbon fiber components.

Sketch4 is a 3D sketch.

Research the BORN Technique... ...works in ANY CAD software.

Understood. (You'll be happy to know your video is at the top of google for this.)

Edit Sketch7

Click and drag line and line endpoints. What do you observe?

I did misspeak in saying that sketch7 was experiencing the same issue. It was experiencing it so I decided to revert to a mostly unconstrained version as I knew it would undergo corrections/redesign later.

Why are there 3 lines here when one line would suffice?

Why, oh why is a rectangular peg used to create a cylinder?

Add a Centerline to the rectangle and Revolve instead

Definitely a silly error in retrospect!

Or Origin is not in an optimal location.

Model with Symmetry about the Origin will save lots of work.

The reason I chose to set the midpoint right below the first gimbal motor is due to the rest of the drone that will be designed above it. Once the rest of the drone is modeled that location will be roughly the center of the entire design. (I'm guessing this was still an incorrect decision?)

Is Body3 correct?

I would expect this to be multiple bodies (and eventually converted to Components with Joints for motion on DoF).

It's definitely incorrect. I'm not sure why, but when I extruded sketch7 it put the majority of the body into body3 with the other arm. I didn't notice this immediately because I was unaware that it could even happen.

[TheCADWhisperer]

@mowen34 

On your Extrude12 - I suspect that you intended New Body rather than Join...

[TheCADWhisperer]

I made some mistakes in the Attached, let's see if you can find them...

[TheCADWhisperer]

@mowen34 

Where did you go?

I consider my first attempt at simply an exercise in understanding the geometry.

Now that I understand the geometry I can simplify even more from my initial attempt.

But there is no point in me making additional effort if you have given up on learning Fusion 360.

[mowen34]

flaws I think I've found:

- The offset face for the hole used for the peg (It also visually appears misaligned, guessing that's related?). It should be dimensioned and revolved from sketch 2 instead.

- The extraneous hole created behind motor 3 in sketch 2 should be removed. 

- Motors 2 and 3 are sketched but the sketches are not used, instead the motor bodies are copies of motor 1. These copies should be deleted and the motor bodies should be made by revolving the sketches.

The rest of the 'flaws' (major differences between our sketches) I can find are simply omissions from my original design.

[TheCADWhisperer · Accepted solution]

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@mowen34 wrote:

flaws I think I've found:

- The offset face for the hole used for the peg (It also visually appears misaligned, guessing that's related?). It

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The offset face was to allow clearance between moving parts - but it was misaligned.

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@mowen34 wrote:

flaws I think I've found:

- The extraneous hole created behind motor 3 in sketch 2 should be removed. 

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In my revision I did not take the time to add the mounting holes in arms and motor.  Use Pattern Feature.

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@mowen34 wrote:

flaws I think I've found:

- Motors 2 and 3 are sketched but the sketches are not used, instead the motor bodies are copies of motor 1. These copies should be deleted and the motor bodies should be made by revolving the sketches.

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No, no, no.

The motors are all the same - so model only one and copy the Component.

I made mistake of using different dimensions for the 2nd and 3rd motor sketches - but it turns out I didn't need to sketch these at all.

I didn't convert the bodies to Components and add the Joints in my Revision file.

When you add the Joints you will probably want to include Joint Limits.

@mowen34 

Ask questions if (when?) you run into trouble.