Helical holes pattern in tube. Is there a better way to do this?

[janus2]

I managed to create this part. 10 holes every 36 degrees at the same distance and size.
But I need 10 Planes, 10 Sketches, 10 Dimensions, 10 Extrudes, ....

I wonder if there is a better way. Just in case there are 100 holes next time.

Jan

[JDMather]

Curve driven pattern is much easier.

Oops, I thought  I was on the Autodesk Inventor forum.

Attach your file here for demonstration of the technique.

[janus2]

Here's the file. There are actually only 9 holes, but it shouldn't matter for the example.

Jan

[g-andresen]

Hi,

pattern on path should be your friend.

1. Create a helical element and place a hole at the starting point.
2. multiply this hole with „pattern on path“
(Options: align to path and optimized)

günther

[JDMather]

---

@g-andresen wrote:

Hi,

pattern on path should be your friend.

1. Create a helical element and place a hole at the starting point.
2. multiply this hole with „pattern on path“
(Options: align to path and optimized)

günther

---

Can you demonstrate how to make this work in Fusion 360 (file Attached - edit as needed)?

[g-andresen]

Hi,

Right now, I don't have access to Fusion. I will not be able to create an example until Monday at the earliest.

günther

[chrisplyler]

Good luck trying to use Pattern on a Path along a helical path. It twists itself in a way that is undesirable. You can correct a Sweep along a helical path by using a second helical path as a guide rail, but there is no ability to do the same for a Pattern on a Path.

[davebYYPCU]

Probably not quite as tedious as the OP's original effort, but you can get the spiralised holes with Pattern on a (coil) Path, if you put in the effort.

Requires a Swap from Solid to Patch and back again, 

credit to this video for parts of the method.

Might help...

[laughingcreek · Accepted solution]

It's really disappointing that there isn't an easy straight forward way to do this in fusion.  The pattern on path command is all but useless for non-planer paths.

@davebYYPCU solution is good, but does produce tapered holes instead of a hole with parallel sides (like you would get from a drill bit)

While still not a good solution, you can save your self the step of creating all the construction planes by extruding a polygon and placing the sketches on the faces.  Below is a screen cast demonstrating doing that.  I also made all the circles for extruding at one time and copies/pasted them into each sketch just to save time.  that probably wouldn't work for your example b/c it looks like the circles would overlap.

[davebYYPCU · Accepted solution]

Tapered holes... Oops, didn't even check that.

Between posts, I remembered this thread, for a Spiral Pattern Script, 

works on Components, and works for a pattern of cylindrical cutters.

When using Combine Cut, select the bodies from the window, no need to keep the tools.

Settings are -18.4mm and -36 degrees (Took a few goes to get right direction.)

Might help....

[janus2]

Thank you all for all your efforts and help.
There does not seem to be a simple straightforward solution.

The solution with the polygon is an improvement over Planes.

The solution with the script seems to be interesting.

I will give it a try, if the next part has more than 10 holes .

Thanks again for the help
Jan

[MichaelT_123 · Accepted solution]

Hi Mr Janus2,

You have had brought a lot of attention to a seemingly simple problem, and rightly so.

Such a structure/topology is quite prevailing in engineering. It requires (obviously) placement of holes (or other features) in the equal distance along linear and radial dimensions. In essence, we have here 2D pattern. Fusion 360 offers two separate ounces, rectangular and circular. The mixed/universal one is not available in F360, and it is a pity as it would greatly simplify and universalize this kind of operations.

Would it be possible to replace the current two rectangular and circular pattern with a universal one UI?

This is a question for TF360,… particularly during a time when a kettle of the new interface is boiling.

Bellow is mine F360  parametric implementation of the helical holes (features) problem.

Note that a universal pattern would replace (on the design’s timeline) multiple of entries there.

Video addendum:

https://a360.co/2JJnN5o

Regards

MichaelT

[janus2]

Hello, Michael!

A really interesting solution. the community here is very creative.
We should not give up hope that Fusion 360 will one day have a suitable functionality.

Thank you
Jan

[ksAZ3XE]

still nothing in 2025 to solve this issue