Extrusion appearing in wrong location

[jvconway_xelera]

Lately, I have been encountering an issue where I try to do an extrusion or revolve that is located somewhere in space and the extruded solid shows up at the origin rather than where the sketch defines it.  In this case sometimes the solids don't even show,  just the outline when you hover over them in the tree. 

[blandb]

Your work plane 1 (Asml tool_3) is 233,366.25879 mm or (~765' 7") away from the origin. Is this correct?

[jvconway_xelera]

That is correct

[JDMather · Accepted solution]

---

@jvconway_xelera wrote:

That is correct

---

In that case - then I would model the geometry at the origin (or within +/-100,000 cm cube of the origin) and then Move the geometry.  Will this be an assembly of components or will it be one massive component.

[jvconway_xelera]

It will be in an assembly. I was trying to model in place in the assembly but wasn't aware of the limitation being so far from the origin.  I typically place my new part origin at the origin of the assembly, but I can place it closer to where I'm working and sounds like that might solve my problem.

[johnsonshiue]

Hi! Just to correct the range, it is +- 100m in each direction within a part. In an assembly the limit is more complicated. If the geometry is created at the assembly level (assembly sketches or features), the same rule will apply.

Many thanks!

[BDCollett]

---

@johnsonshiue wrote:

Hi! Just to correct the range, it is +- 100m in each direction within a part. In an assembly the limit is more complicated. If the geometry is created at the assembly level (assembly sketches or features), the same rule will apply.

Many thanks!

---

Hi Johnson. 
Has there been a regression with this for 2024?

I have someone who has just upgraded from 2023 to 2024, they have a derived sketch from a point cloud that has features over 100m away from the origin. It worked in 2023, in 2024 it now does not work consistently.

Saying "just don't model over 100m away" is hard to suggest when it has been working fine for numerous years.

Edit: Testing 2023 vs 2024. There is definitely a regression here. Funnily enough, if you open a file created in 2023, it works in 2024, create new sketch geometry and it doesn't.

[BDCollett]

I have attached a model, created in 2023. Saved in 2024.1.1

The outer square was created in 2023, you can see that it can be moved anywhere, and the extrusion feature will work.

The 20m square, as soon as that is moved past 100m, it fails. This was a new sketch and extrusion feature added in 2024.

20m square inside 100m:

20m square outside 100m:

Would love an explanation of what is going on here. I suspect it's a 'spaghetti code' moment.

[BDCollett]

@johnsonshiue sorry to bump this again and I know it's 'solved' but can we get some input onto the regression? 

[johnsonshiue]

Hi Ben,

This is indeed a bug in 2024. We do have a fix targeting the future release. I am not sure if the same fix can be applied to 2024. I need to work with the project team to understand it better.

Many thanks!

[BDCollett]

---

@johnsonshiue wrote:

Hi Ben,

This is indeed a bug in 2024. We do have a fix targeting the future release. I am not sure if the same fix can be applied to 2024. I need to work with the project team to understand it better.

Many thanks!

---

Thanks for the reply. 

It is honestly bugs like this that make customers scared to upgrade their software. There is always the risk that something completely breaks their way of working and the answer is "sorry wait until next year".

[johnsonshiue]

Hi! I have worked with the project team and understood the fix better. The fix is portable but it has to be versioned. For existing 2024 files with the missing extruded body, the extrusion will need to be deleted and recreated with the fix (supposedly in 2024.2). Then it should work.

Inventor as any engineered products can have bugs and regressed behaviors. We do try avoiding the bugs but from time to time, things can slip through the crack. I am very sorry.

Many thanks!

[tonmoy5KZPE]

I am also having the same issue of extrusion error (created somewhere else away from sketch plane) where my X = -127560 mm and Y = 00 with Version 2024.1. It seems the extruded component is created at 0,0 strangely with error message. Like to know the roundabout solution because my design is for ducting deriving from skeleton sketch. When the new update (2024.2) is expected.

Thanks

Tonmoy

[johnsonshiue]

Hi! 2024.2 will be available sometime in October. A testable patch may be available on Inventor Feedback Community a few weeks before that.

Many thanks!

[hithere8]

I am have the problem. 

It is a large dim ipt file. The extrusion appears far away from its matching location on the sketch. Frustrating...

[hithere8]

Here is a screenshot, the yellow part is the extrusion for the blue sketch area

[tonmoy5KZPE]

Hi
It was also frustrating for me as well. Inventor 2024.1 works only
between +/- 10000 units from origin (0,0). Beyond that this version has the
problem it seems. I had to redo the project again in version 2023 and had
no issues yet. In the process lost a lot of man hours causing delay in
delivery. Autodesk, I presume, has to provide an update with the fix.
Thanks

[johnsonshiue]

Hi! I am very sorry to hear that 2024.1 isn't working for you as it should be. This particular issue is a combination of a preexisting issue and a regression defect. It is specific to 2024 and 2024.1. The fix has been implemented in the coming 2024.2 update. If you still have files with the erroneous behaviors in 2024.1. Once 2024.2 becomes available,  you may go to Manage -> Rebuild All to recompute the features and they will work correctly beyond 100 meters. However, the valid model range is still +-100m in XYZ. Going above +-100m a bit (like +-200m) might be Ok. +-1000m will destabilize the model for sure.

Many thanks!

[BDCollett]

2024.2 is out. Can confirm after doing a rebuild that it seems to have fixed this issue.

[hithere8]

Thanks very much. Will try it out soon.