Pattern along a 3D curve or geometry in assembly

[MikeLA7KX]

Im trying to pattern along a piece of gemotry in an assembly and having trouble. Can anyone advise the best method for this as i cannot get it to work. I would upload the files but they are pretty large.

I have attached an image. At the moment my circular pattern is based off the axis, however the spiral also goes up which i am unable to replicate in a pattern.

I have tried various patterns in a part and assembly and still cant figure out how i can achieve what i want. I basically want the first part to pattern around the curve.

TIA

[CCarreiras]

HI!

I would create a coil in a part and create a pattern thru the coil geometry.

In assembly, select the part pattern to create an assembly pattern.

[MikeLA7KX]

Thanks for your reply but i cant get it to work.

It wont let me pick the geometry in an assembly.

A pack and go is about 1.1gb so dont really want to upload.

[JDMather]

@MikeLA7KX wrote:

A pack and go is about 1.1gb so dont really want to upload.

---

You are probably using the wrong settings and including a bunch of extraneous stuff, but if it really really is that large - then simply make up a small dummy assembly that exhibits the desired behavior.

[MikeLA7KX]

No the file is big.

It has a .iam that has been saved from a .sat file so has 1000's of parts.

Ive attached the coil part.... I have put that part in to my assembly. Cant select any geometry.

[JDMather]

---

@MikeLA7KX wrote:

Ive attached the coil part.... I have put that part in to my assembly. Cant select any geometry.

---

You did not Attach your assembly *.iam file here.

You did not Attach the *.ipt file of the Component that you wish to Pattern.

Your Coil part file works fine for me when I place into an assembly and attempt a Component Pattern, but I would have done your Coil differently.

First I would have fully constrained Sketch1.

I would have used a simple line rather than a circle such that the result is a surface body rather than a solid body.

Change your Browser to Modeling rather than Assembly, and then you can select your Rectangular Pattern from the Coil part directly in the browser.

[johnsonshiue]

Hi Mike,

Are you trying to pattern assembly feature along 3D curve? Or, pattern components along 3D curve? These are two totally different workflows.

Many thanks!

[MikeLA7KX]

Im trying a couple of things which i think im getting confused with.

Im trying to pattern along the 3D curve (the coil) which i have kinda done in one part file.

I then need to use that coil geometry to pattern other parts in an assembly.

The advice above still doesnt work when switching to modeling tab in an assembly. I dont have any patterns in the assembly which i assume is why it doesnt work.

[MikeLA7KX]

Nevermind - can actually select the patterns now! weird..

[JDMather · Accepted solution]

---

@MikeLA7KX wrote:

I don't have any patterns in the assembly which i assume is why it doesnt work.

---

I guess you have figured this out, but the pattern is not in the assembly.

In the image in Message 7 you should see that I drilled down to the part level within the assembly browser to find the part level feature pattern.  It is a bit hidden workflow, but works every time.

[Tom_Sturtevant]

JDMather is correct that you need to select the part’s pattern in the browser in this case because the pattern only contains work features.  If the associated part pattern has real geometry you can select it in the scene (or in the browser).

One other tip – if you want the Assembly pattern occurrences to be oriented based on the curvature of the path you need to specify Orientation = Direction1 in the extended portion of the pattern dialog when creating the part level pattern of work points.

Hope that helps!

T.0.M.

[Hunteil · Accepted solution]

Bravo! This is exactly what I was looking for!!! 👏
This was extremely hard to find btw guys. Me and the guys at my company have been looking for this solution for over a year and kept coming to solutions using other methods that don't meet our needs. This is perfect for Spiral stairs & similar structures like that. I want to also say this method was crazy hard to figure out until I found this. I was actually hunting for an Idea post for easier patterns for helical / spiral assemblies at the assembly level instead of at the .ipt. I guess this will do lol.

Solution for TTLD folks:

1. Make .ipt, create 3d Sketch.
2. Place Helical Curve.
3. Finish Sketch.
4. Place Work Point at start of Helical Curve.
5. Use Pattern>Rectangular.
6. Select curve. Expand the arrows. Pick Compute, Direction, and Orientation as needed. Mainly if you want the part to rotate as it rotates around the spiral rise / pitch / revolution.
7. Save and create a new .iam.
8. Place the new .ipt w/the pattern inside it.
9. Place another part that you want to pattern.
10. Constrain to the very first point. (you can apply more later.)
11. Click the Pattern tool.
12. Now the tricky part. In the Assembly browser like message 7 shows from JDMather. Click the Modeling button to display all the modeling features for each component.
13. Click the Pattern you want to follow. (Again as shown in message 7.)
14. Done that's it! Not much you can do in the assembly for editing the pattern. The modifications will need to happen at the .ipt file per step 6.

I hope this helps others also confused on this topic. Thank you @JDMather .

If anyone wants to vote on a possible improvement, please check out this idea: https://forums.autodesk.com/t5/inventor-ideas/spiral-helical-curve-pattern-in-assembly/idi-p/1219407...

[rwilliamsCL9QS]

Thanks for doing the work on this.  I was able to utilize this to show products flowing up/down a spiral conveyor, and your instructions got me there.