Sketch Driven Pattern Orientation

[nicholas_provo]

Hi

Got an issue with the orientation of a sketch driven pattern.

I got 3 sleeves extruded on a vertical panel and I want them patterned on a horizontal panel.

Put a new sketch on the horizontal panel with the points.

Selected sketch driven pattern, added the features, added the sketch with the points and clicked faces on the horizontal panel.

But the orientation does not change, it keeps the original orientation of the vertical panel.

To add: this is a multi body part.

Any Ideas what I am doing wrong?

grt
Nicholas

[johnsonshiue · Accepted solution]

Hi! Unfortunately, Sketch Driven Pattern does not offer orientation control. If you need a different orientation, you might need to create another feature and pattern as such.

Many thanks!

[nicholas_provo]

Ok

Then I'll stop searching, thats one for the Idea Station!

[fsanchou]

@johnsonshiue,

Hi,

What is the purpose and how to use this Face button ?

Thanks,

[torbjorn_heglum1]

You can use the face button to orient the instances of your sketch driven pattern.

- Select a face where the original feature is placed, and corresponding faces for the rest of the instances

- if no such faces are available in the real model, I normally create an additional  surface for this purpose

The picture below shows a bracket in a master model that is patterned with variable distances and orienation.

On the detail below you see that the orientation id changed, as wanted.

Works quite well, but bugs out some times where faces are 90 deg on each other, the instances can flip 180 deg.

Torbjorn

IV2017.4

[DGiandomenicoMS5XW]

I am encountering this same issue with Inventor 2024 that was reported in 2018.   A single instance, at 180 degrees of the original, is flipping upside down.

[johnsonshiue]

Hi! The behavior could depend on the geometry. If possible, please share the files in zip with me directly johnson.shiue@autodesk.com. I would like to understand the pattern orientation issue better.

Many thanks!

[Dormis8749]

Was this problem fixed? I'm also experiencing an instance that flips 180 deg.

[CGBenner]

@johnsonshiue Do you know if there has been any change regarding this behavior?

[johnsonshiue]

Hi Marius,

I am aware of an issue that could lead to the last instance flipping. This is indeed a known issue, INVGEN-75057. The latest status shows that it has been fixed on an internal build targeting the future release. Unfortunately, the fix cannot be ported backward due to the migration requirement.

Many thanks!

[nathan_wostrel]

I am still seeing this behaviour in IV2024.3.3  Is the fix going to be in IV2024, or do we need to wait for IV2025?

[ObradKostadinovic]

I have the same issue in 2025 (updated to the current last version). It's hard to reliably reproduce the issue, or understand what is the cause. I have an upgraded problem too, where all instances simply stick to the first orientation, no matter the faces I select. Wonder if it's working in 2026? This kind of makes the sketch based pattern unusable for me.

Not working in 2026, the pattern simply doesn't respect the face orientation

[johnsonshiue]

Hi! Could you share your example with me directly at johnson.shiue@autodesk.com? I would like to understand the patterning behavior better.

Many thanks!

[kacper.suchomski]

Hi Obrad

This has been largely fixed in version 2026:

https://youtu.be/YN47vGqcnm0?feature=shared&t=472

I also recently developed such an element using a sketch-driven pattern with orientation:

Can you share your file or a similar file reflecting the behavior?

[ObradKostadinovic]

Hi Kacper,

I tried editing the file in the latest 2026 but no luck. This is just a plain extrusion and an extrusion cut that I want to pattern. Parts are derived from a master, they are all similar and the sketch pattern works on some and fails on others like this one. I'm a bit stumped since there is nothing at all that I can even change, except maybe creating my part using a sweep? But then again this works on some parts and fails on others. Still trying to work it out.

edit: after placing the pattern sketch directly on the part (the sketch was offset from it) I get a better result, although it's still broken, as you can see in the other image.

Oh, and your part reminds me of gridfinity, is that something that you will print?

first try with offset pattern sketch

pattern sketch created on the part, random rotation on one face (the others are fine)

[kacper.suchomski]

This was a base for connecting the boards so they wouldn't slide relative to each other during play. My client prints it and sells it.

I tried to reproduce your problem and... it works for me.

I specifically defined different spacing between occurrences so that it wouldn't be possible to do it with a circular pattern.

There is a chance that you are using the tool incorrectly or missing an important step in preparing the pattern guidelines.

Are you sure you have read all the guidelines and requirements for using Sketch Driven Pattern?
You can read my comments in this thread:
https://forums.autodesk.com/t5/inventor-forum/inventor-2026-sketch-driven-pattern-of-a-hole-in-a-par...

Let me know how it goes.

If the problem persists, please provide the file for analysis.

[ObradKostadinovic]

Yeah I can make it work if I make a new part, the problem is that I have a bunch of derived stuff. Here's my part with a suppressed source - no idea if you can open it without issues.

I'd like to know why it happens but I can't supply the master part.

And I guess another solution is to link the parameters from the master file and create the sketches in the derived part, which I wanted to avoid. If that works I'll let you know

[kacper.suchomski · Accepted solution]

So:

As I mentioned in the article, sketch construction points should not be used as a locator for base geometry. This practice is inconsistent with the algorithm and exposes the user to geometry duplication, which can result in, for example, incorrect bolt insertion in the model and incorrect component counting in the BOM.
Please read carefully the statements in the link I provided.

Reference geometry serves sketches. It shouldn't exist in a vacuum. It must be compatible with the sketch so that Inventor can identify specific directions for specific instances.
If you meet these conditions, everything will be fine.

[ObradKostadinovic]

Thank you, this helps a lot. I still think autodesk has huge issues with UI and communicating with the user, and I still think it's really strange that this sometimes works if I do it my way, but I'll change the way I create the sketches and remember this. I guess the pattern works if you happen to run into Kacper, otherwise you're stuck.

edit: I still have this issue, randomly, even when I replicate your workflow completely. There must be some problem with the derive, but since there is no clear solution I'll try with exporting parameters and recreating parts based on that.

[kacper.suchomski]

No, it's not a derivative issue.

As I showed you in my first reply, the opposite surface issue has been fixed in version 2026.

You need to delete the command created in the previous version (defining positions the old way) and create the pattern in the latest version.

There are reasons why parametric 3D CAD programs lack backward compatibility.

You just experienced one of those reasons firsthand.

Update your software and enjoy the new features.