Basic questions about circular feature pattern

[theycallmevirgo]

The attached assembly contains part "neoprene". Feature "Stitch" in "Neoprene" is constructed from a sketch on a plane tangent to the revolved Sketch1. Pattern "Stitches" is a circular pattern along the projected construction line on the offset plane around the constructed axis. Then I mirrored it across the perpendicular plane. 

My initial goal was to offset the first "stitch "by a given distance from the "start" of the revolved body and space evenly. I decided on this technique after watching some YT videos. Is it "correct"?

Is there any way to input arc length distance into circular pattern, or will I have to do something clever with Pi/trig/inverse trig?

Thanks so much 

Joe

[cidhelp]

Hello @theycallmevirgo ,

do you want to use the arc-length (on base cylinder) as distance for the holes?

I would sketch an arc for the holepattern and create an arc-length dimension. After creating the first hole, you can pattern (rectangular pattern!) along the arc-path.

 

[SBix26 · Accepted solution]

Several things that would make this simpler for you:

• Make the X-axis the center of the first Revolution feature so you can use it for subsequent features (not easily corrected in this file due to adaptivity)
• Instead of creating the Stitch feature as a circular Extrude/Cut, use the Hole feature
• Holes can be located by a point (location) and axis (direction), so no need to create lots of workplanes
• Feature patterns have a Midplane button to make the pattern symmetric

I've attached a modified file (2025 format) for you to look at.  Here's the Circular Pattern feature I used showing the Midplane control:

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Sam B

Inventor Pro 2025.1 | Windows 11 Home 23H2

[theycallmevirgo]

"do you want to use the arc-length (on base cylinder)" 

Yes, that's it exactly. I'll try your approach shortly.

[theycallmevirgo]

Why do you say using hole reduces the number of workplanes? I'm still using the one offset plane to define the pattern the way I did it originally.

[SBix26]

Because Hole location and direction can be defined by point and axis, so a sketch is not required.  I used your Sketch2 to define the workpoint and workaxis for the Hole feature, so no further workplanes or sketches required.

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Sam B

Inventor Pro 2025.1 | Windows 11 Home 23H2

[SBix26]

Here's another pattern method which is probably even better for your purposes.  I constrained an arc centered on the projected edge to be the direction for a rectangular pattern, and dimensioned the start point from the edge.  In the pattern, I specified the number of instances and that they be distributed evenly along the curve.  No calculations or arc length dimensions required.

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Sam B

Inventor Pro 2025.1 | Windows 11 Home 23H2

[theycallmevirgo]

Sorry, but I'm still unclear. Both your technique and my technique use a plane offset from the face created by the revolution, on which we make a sketch from the projected cut surface. What additional planes does my technique use?

[theycallmevirgo]

Also - in SBv2 is d24 a linear distance, or an arc length? If a linear distance, do you know how to make it an arc length?

ETA NVM I figured that part out

Thanks again 

Joe

[theycallmevirgo]

Also, why is the sketch feature line that defines the hole not a construction line? Why does the part break when I make it a construction line? 

Thanks again 

Joe

[theycallmevirgo]

The real problem is, I don't really want to input number of instances for pattern command. I want to do it by arc length spacing and total distance.