Rectangular pattern won't align hexagons

[Anonymous]

Hi Support,

Fusion will not align a hexagon of 7.1mm side length when doing a rectangular pattern, for either in sketch or body.  If I change the side length to 7.101 it aligns correctly and objects can be combined.

[wmhazzard]

Please attach an f3d file of your model to a reply. 

[Anonymous]

f3d attached along with 2 screen shots showing 7.1mm and 7.101mm

[Anonymous]

Screenshots of before and after and f3d attached

Form the screenshots you can see the only difference is the change in hexagon side length.  One carries over correct spacing for bound areas, the other does not, and you can't even force align the points.

This was a simple blank project.

[davebYYPCU]

Sketch bug to show you why modelling patterns are more robust and sketch pattern is not recommended.

Same pattern - modelling is correct due to the successful Combine, if that same problem was evident in the modelling pattern, the combine would spit the coincident faces error out.

Might help....

[Anonymous]

But even if I create a body from the single hexagon and do a rectangular pattern for the body at 7.1mm, the same problem exists.  I can't combine because the faces are not coincident.

Screenshot attached

[jeff_strater]

Maybe I am missing something here, but don't you have to make the pattern spacing dependent on the polygon side length?  You have the pattern distance at a constant 12.898, but the correct distance will depend highly on the hexagon side length:

To see that, go bigger, say, to 8.  You still have the same 12.898 for the pattern distance

[davebYYPCU]

@ 7.1mm my body pattern did not fail.

You new pic does not say anything.

@jeff_strater the sketch pattern does not find the border profile. (black dots)

Might help....

[jeff_strater]

I think that is because there are two points here:

and, they are not quite at identical coordinates

I think that is because that 12.898 distance may not be exactly the correct one.

[davebYYPCU]

I use 3 decimal places, your measurement has 3 leading zeros, should be 3 coincident points.

regardless the modelling pattern and combine worked here.

[Anonymous]

Correct

[Anonymous]

You're onto it.

How does Fusion detect the spacing if you don't manually enter it?  I always select "Measure" and it seems to work it out.  When I select "Measure" it doesn't space correctly.  Is there an auto-spacing feature so that its not hard measured?

[Anonymous]

You found it.  That is exactly the problem.  Fusion bounds the original hexagon correctly, but when it patterns, the points no longer coincide.  If I add 0.001 to the hex side it patterns correctly and bounds the replicas.  

[TrippyLighting]

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@Anonymous wrote:

You found it.  That is exactly the problem.  Fusion bounds the original hexagon correctly, but when it patterns, the points no longer coincide.  If I add 0.001 to the hex side it patterns correctly and bounds the replicas. Real

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 LOL!

The mathematical formula to calculate the amount of movement for the pattern instance is:

(side_length * sin(30) + sketch_offset) * 2

If you plug that incredibly complex mathematical formula into the pattern field and reference the parameters for the dimensions you used in the sketch it looks like in the screenshot below and surprisingly it works and is fully parametric.

 

[Anonymous]

So can you replicate the problem or am I seeing stars? 

[TrippyLighting]

What do you see when opening the file I had attached ?

If you had used "all digits" when copying the measured value you'd see the same result and there's no problem.

3 digits accuracy is OK for manufacturing purposes, but in this case you'll have to adhere to the precision the CAD system requires to operate properly. 

[TheCADWhisperer]

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@TrippyLighting wrote:

If you plug that incredibly complex mathematical formula into the pattern field and reference the parameters….

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In Autodesk Inventor Professional - I use Reference (driven) dimensions (fully associative parametric) for stuff like this.  Too bad that can’t be done with Fusion 360!  🤯

Now, back to the show…

[TrippyLighting]

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@TheCADWhisperer wrote:

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@TrippyLighting wrote:

If you plug that incredibly complex mathematical formula into the pattern field and reference the parameters….

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In Autodesk Inventor Professional - I use Reference (driven) dimensions (fully associative parametric) for stuff like this.  Too bad that can’t be done with Fusion 360!  🤯

Now, back to the show…

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Yep, that would indeed be nice, but on the other hand, in this case that little bit of middle school trigonometry shouldn't be too difficult.  

[Anonymous]

Are you saying its a rounding error due to 3 decimal point spacing?

[TheCADWhisperer]

@Anonymous 

Before I jump into this discussion - are you sure that you want to dimension your hex as you have done?

With calipers (or other measuring instruments) it would be very difficult to measure that 7.1 distance with any accuracy in the real world.

Normally we dimension hexagons across the flats (think of your standard hex head fasteners or mating wrench or socket tools).

Do you really want to control from the length of that line or would it be better to control across flats?

(Either way is OK, but is one way better than the other?)