How to create a sketch driven pattern in an assembly?

[Anonymous]

Hi,

I'm trying to create a 'sketch driven' pattern of a part in an assembly. Can inventor do this?

I know I can create 'sketch driven' patterns of features in parts but can I create 'sketch driven' patterns of parts in assemblies?

I'm using Inventor 2017

Thanks

[Anonymous]

What exactly are you trying to achieve?

My first guess would be to reference the pattern dimensions to the corresponding dimension in the sketch

[JDMather]

Easy to do.

Attach your assembly here.

[Anonymous]

You'll need to create work points in the part file itself using the rectangular pattern tool. You can create a path or curve to place your work points as needed. Then when you're in the assembly, switch over to model view and reference the part's rectangular pattern to pattern your component.

---

[JDMather]

The OP indicates using r2017.  There may be new functionality for this purpose (will know when actual design intent (the files)) are posted.

[Anonymous]

Thanks for quick replies everyone. I'm new to the forum, how do I reply to multiple posts in one post? (a nice problem to have)

To clarify:
I have a jagged mullion and I want to pattern spigots up the side of it. However, I want to pattern them along a jagged line. To do this I thought I could create a sketch composed of points which indicate where I want the spigots to be, then use a "sketch driven pattern" command to propagate the spigots.

@Anonymous

"What exactly are you trying to achieve?

 My first guess would be to reference the pattern dimensions to the corresponding dimension in the sketch"

See above.

@Anonymous

"Easy to do.

Attach your assembly here."

Can you recommend an easy way to send assemblies with all the parent/child links intact? I read the following guide:
http://cadsetterout.com/inventor-tutorials/copy-an-autodesk-inventor-design/#copy-design-sdk

I tried pack'n'go but it carried all my template files, which seemed unnecessary.

I tried the 'copy' command from the assemble tab and copied the assembly and the parts to a new folder but it only had a 16kB lock file in the folder.

Then I gave up and took screen shots.

@Anonymous

"You'll need to create work points in the part file itself using the rectangular pattern tool. You can create a path or curve to place your work points as needed. Then when you're in the assembly, switch over to model view and reference the part's rectangular pattern to pattern your component."

Hi Jacob, unfortunately the work points which I want to follow are not in a rectangular pattern, they're all jagged and at different distances apart too. It will be much faster for me to locate the parts using a sketch rather than constraining every part in three dimensions.

I see from your screen shot that you've created a curved pattern of balls using a rectangular pattern. Did you create a rectangular pattern then 'redirect' it along a sketch? I tried to follow you but I'm missing something.

Here are some screen shots of my attempt in a simplified model (far less parts to pattern). I have the part in the assembly (the cube/spigot) which I want to pattern and I have a sketch to indicate the multiple points where I want to pattern the part on to. However, I can't select the spigot as a feature to pattern using the "sketch driven" pattern command.

I can create a sketch driven pattern of a feature in a part but I don't want to do that. I want to create a sketch driven pattern of a part in an assembly.

Any ideas?

[mdavis22569]

picture from his post ... 

(I had the wrong idea)

[Anonymous]

Hi mdavis,

Yeah I saw that one but unfortunately that's for patterning a FEATURE in a PART.

I need to pattern a PART in an ASSEMBLY.

[mdavis22569]

sorry ...looking at it in the smaller pictures I didn't pay attention to the browser ..my bad.

however looking at the picture it looks like it would be a feature ...

Just tried a multi body ..that's not an option ..

[SBix26 · Accepted solution]

Create a sketch-driven pattern of workpoints in one of your part files, then constrain a spigot where you want it and pattern it using the feature pattern from your part file.

Pack & Go is the way to post an assembly here.  You just didn't notice the various options you have for what to include-- there are check boxes for templates, libraries, etc.

Sam B

Inventor Professional 2017 R2
Vault Basic 2017
Windows 7 Enterprise 64-bit, SP1
Inventor Certified Professional

[JDMather]

---

@Anonymous wrote:

@Anonymous

"Easy to do.

Attach your assembly here."

Can you recommend an easy way to send assemblies with all the parent/child links intact? ....

I tried pack'n'go but it carried all my template files, which seemed unnecessary.

---

[Anonymous]

@SBix26

Sweet. That worked. Thanksbixler. Patternception.

@JDMather

Ahh, yep. I'm bad. Should've noticed those check options. That'll be handy for next time.

Appreciate everyone's time. Thanks a lot!

[Anonymous]

Yes, it's sort of misleading called a rectangular pattern. You can pattern along a path. See attached screencast.

[Anonymous]

The solution to this post did not work for me.  I created a workpoint pattern in the part.  However in the assembly I am not able to select the workpoint pattern as a feature source for the component pattern.  Any thoughts?

[JDMather]

---

@Anonymous wrote:

...  Any thoughts?

---

Attach assembly here?

[Anonymous]

I've created a simple dummy assembly.  My goal would be to pattern the second part, based on the workpoints in the first part.  

[andrewiv]

It won't let you select the pattern in the graphics window, but you can switch your browser to Model and select the feature pattern from the browser.

[JDMather]

You missed part of the instructions above.

[Anonymous]

This worked, thank you!

[SF8906]

I have Inventor 2019 and I am unable to do this.  The Pattern doesn't show up under the part in the assembly.  Did Autodesk remove this capability?