Tricky Circular Pattern question

[2long]

I would like to make a parametric design for locating spokes on a semicircle (180 degrees).  While it is simple enough to use the partial and angle parameters in the tool, I would like the design to work whether the number of spokes is odd or even.  I don't know where to locate the initial feature to have the pattern work in all cases.

The included design should have 3 spokes.  Each 45 degrees apart with the center one at 90 degrees.

Any hints would be welcome.  First post, so if I should include something else, or present the question in a better way, just let me know.

Thanks in advance

[HughesTooling]

Does setting the angle for the sketched first spoke to angle/2 give what you want? See attached file.

[HughesTooling]

Just some advice on your design.

You should fully constrain your sketch so changes to dimensions are predictable and you don't risk dragging something by mistake!

Add the extra constraints and dimensions so you get the red lock on the sketch for fully constrained.

It is best to avoid symmetry constraints if you can as they are harder to solve and can slow Fusion down. You can usually get a simpler sketch using midpoint constraints.

You should not have unconstrained points in sketches even on construction lines also avoid lines on top of lines.

Your spoke leaves a gap at the end by the way? A midpoint constraint between the construction line rather than using the corner point would fix this gap.

An easier way to draw the spoke would have been to use the 3 point rectangle tool. Then constrained it to the construction line with midpoint constraints.

Not sure how wide you wanted the spoke, it was around 2.6mm?

Here my simplified fully constrained sketch. I noticed you had the display of constraints disabled, probably not a good idea until you have a better grasp of sketching in Fusion. See attached file.

[2long]

Mark,

Thanks so much for the constructive feedback.  I was lazy with the file I attached in just wanting to get the idea out there.  You suggestion about using the 3 point rectangle really helped, although I struggled for about an hour figuring out how you did it.  For anyone else fighting with it, this was my technique.  I started the rectangle well away from either of the arcs in the drawing.  The second point was placed when the parallel constraint snap (to the construction line) showed up.  Lastly I used a dimension to fix the width of the spoke.  Then I selected the intersection of the construction line and the outer arc, selected the midpoint constraint and then the side of the rectangle closest to the arc.  Lastly, I selected the coincident contstraint to fix the corner closest to the inner arc and the arc itself.

As to the original question (sleeping on things can really clear the mind), I came up with this solution.  The computed angle between spokes is 180 / number of spokes + 1.  This was key to getting the first spoke computed in the sketch correctly.  Then in the circular pattern, the angle is 180 - computed angle * 2.

I welcome additional feedback on my technique.  I am really enjoying learning all about fusion 360.

[HughesTooling]

I noticed a small error on the part where there's a line that should not be there.

I traced this to a small error in the first sketch.

I'm not sure how you've got this error and still have a fully constrained sketch. It might be because you've created the part very close to the origin and when you added the midpoint constraint Fusion has seen it as in tolerance so doesn't move the midpoint of the line to 0,0. @jeff_strater what do you think? (EDIT I figured this out, see next post)

What I did was delete the midpoint constraint, dragged the line away from the origin then applied a coincident constraint between the origin and the circle centre.

Although I'm not sure what is constraining the circle centre to the midpoint of the line at this point as no constraint is showing!?

Anyway after adding the coincident constraint to the origin the model look good. See attached.

[HughesTooling · Accepted solution]

I see now what's keeping the circle centre at the line midpoint is the 2 dimensions in this sketch.

Odd way to do this as one dimension and a midpoint constraint would do the same and be more obvious how it works. Might be why you ended up with the small error. There where a lot of stacked points here and hard to unpick which point is constrained to the origin and which points are constrained to other points. I've seen this sort of problem before when there's a stack of points on the origin.

[2long]

Thanks, that is a better solution.  I have found it difficult to find what is under- or over- constraining my sketches.  That was one of the reasons why in the original post I had turned off the showing of constraints as I was just confused by them all.  But what I think I have learned is to watch the sketch lock icon after every change to see if I loose full constraints.  Is that a good strategy, it seems tedious when you are in the flow of drawing.  Is there a better way?

[HughesTooling]

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@2long wrote:

But what I think I have learned is to watch the sketch lock icon after every change to see if I loose full constraints.  Is that a good strategy, it seems tedious when you are in the flow of drawing.  Is there a better way?

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It's hard to have a rule for all situations but what I do is sketch the shape roughly with no dimensions. You will get some constraints automatically like horizontal\vertical, parallel\perpendicular etc. Then add this minimum amount of dimensions and constraints to fully constrain. If you add constraints and dimensions as you add each element you'll probably end up with an inefficient sketch with too many constraints. The logic of what's going to work best is just something you need time to learn.

[HughesTooling]

@2long An even easier way to do this is use a Thin Extrude so you only sketch a single curve for each part.

So start with a simple sketch like this.

After extruding the centre arc,  use thin extrude to give a width to the extrusion.

Same for the spoke.

See attached file.

[2long]

Thanks for that tip as well.  I hadn't realized that is what was meant by "Thin Extrude" in the dialog.  This makes things much easier.

[HughesTooling]

@2long Are all the segments supposed to be the same size?

The 2 that have horizontal edges are a different size because one edge is offset to one side whereas the spokes are offset symmetrically. Something looked odd but took a while to spot what was different!

[2long]

@HughesTooling They should be.  I am impressed by your attention to detail.  You must do this for a living.  For me it is a 3d printing hobby in my semi-retirement.  I will strive to be more professional in my approach.  I have learned a ton just from your posts.  It is very kind of you to share your knowledge with the community.

Matthew

[HughesTooling]

@2long Yes I do use Fusion for work. While my machines have been running your design was open on my PC and I just came up a few thoughts on the design.

If you look at the last design I uploaded using Thin Extrude you can just edit the first Thin Extrude and change the wall location to centre and all the segment will be the same.

Edit. You might need to change the sketch as well to get the same outside diameter.

[2long]

Yeah, I played around with the thin extrude when you mentioned it and got it working (then when I saw the segment length post, I verified that is was correct).  It was a learning experience fixing all the projections that were lost, but good practice.  I will be calculating the outside arc radius as well as spoke thickness later based on user input.  Ultimately, this will be a peg board attachment to hold screwdrivers.  I thought it would be fun way to learn more about parameterization.