Centered pattern missing some features

[GG_Dynatec]

I am working with some table-driven assemblies. Some of the parts are piping flanges, with cylindrical machining in the mating face. As a result of the machining, when trying to create the corresponding views, the face of the flange, even though looks circular, is made out of either 90 or 180 degrees arcs.

I am trying to show the holes in the flange on a centered pattern but, regardless of how I select the items, there are always some left out. If I try to do the same on the non-machined side of the flange, everything works fine as those lines are actually circles, rather than adjacent arcs.

Since my intention is to be able to produce a unique drawing for each row in the iAssembly (and whenever we come up with a new one) I am looking for a way to create the centered pattern including all the drawing features. Short of superimposing circles over the arches, I have not found a way to do it. 

Any suggestions?

[Lucas.dolinarVFXZU]

The Centerline tool will get a similar result, only difference being the lines dont extend to the center of the pattern.

Centerline > select all holes (midpoint or arc) > select first hole > done

[GG_Dynatec]

Thanks for the answer, Lucas. I am not sure if you meant "Center Mark" as opposed to "Center Line" or not. If not, then can you please provide a little more information about your solution? 

In the case of Center Mark, one of the lines is always vertical, the other always horizontal. In a Centered Pattern, one of the lines is always radial, the other is always tangential. For the holes located at 0, 90, 180, and 270, this does not matter, but it does for all the other ones. 

That being said, I made a test creating a sketch with the same circumference as the flange, then created a Centered Pattern, selecting only the holes orthogonal to the axes. Does not look that bad, although not the solution I am still looking for. 

 

 

[johnsonshiue]

Hi! I suspect this could be a limitation in iPart/iAssembly workflow or it is a bug. Somehow the hole features are not properly recognized. Try this real quick. In the drawing file, go to Tools -> Doc settings -> Drawing -> Default Automated Centerlines. Make sure all features are selected under "Apply To."

If it still does not work, please share the files here. I would like to understand the behavior better.

Many thanks!

[Lucas.dolinarVFXZU]

No, i meant the Centerline tool:

you just need to select the holes in the pattern:

But yeah, something may be wrong in your part, can you share it?

[GG_Dynatec]

Oh, I see now. 

I have an assembly made out of table-driven parts. The assembly itself is also table-driven. 

Some of those parts are plastic flanges. In the assembly, there is machining on the mating side of the flange, created as an assembly feature. When trying to create the centerlines on the non-machined side of the flange, I don't have a problem because all the contours are in the same flat plane, therefore the view is created as full circles, and the tool works without a problem.

On the machined side, however, all the contours are not in a flat plane, but a view-from-the-side cylindrical one. All the lines in the view, although they look like circles, are actually made out of (2) 180 deg arches, or (4) 90 deg ones. That is what is messing with the tool so it is unable to assign a "circle center mark" to something that is not a circle but two adjacent arches. 

Similarly, the centerline tool worked fine on the non-machined side but produced an octagon on the machined side. 

Being this is a table-driven assembly made out of table-driven parts, I am trying to make this drawing works as a template for every single one of the different combinations, just by selecting a different model state in the views. I noticed the problem because I had created annotations in one of the model states but, when changing to another state, some annotations got distorted. That's when I noticed it was not picking up all of the center points. 

A last note. We are switching from another 3D platform and using Vault professional 2021. Since we do not have a lot of files stored in Vault yet, we figured it was not worth trying to update Vault just yet so we decided to defer for one more year. As a result, we are stuck with Inventor 2021 for the time being. 

I attached the drawing and the assembly. 

Thanks. 

[GG_Dynatec]

John, thanks for the answer. 

I made sure all the features were selected and kept on having the same results. Please see the explanation I added on the other thread. The files are also there. 

Thanks. 

[GG_Dynatec]

Sorry, I had attached the wrong assembly file. here is the correct one. 

[johnsonshiue]

Hi! Inventor iam file is a wrapper without geometry. You will need to include all the ipt and iam files (in zip).

Many thanks!

[GG_Dynatec]

Sorry, by bad.

This time, I packed everything into a ZIP file. This should provide all necessary files. 

Thanks. 

[Lucas.dolinarVFXZU · Accepted solution]

Ah, i see. The reason the hole is split on the drawing is that this cut is at 0 Thickness in the middle:

also, This part has a 0 Thickness face:

I cant really explain why it creates the polygon when using the centerline... maybe @johnsonshiue can ask some dev's about that? Also, what i didnt know: these tools are actually the same, just different options:

 

If you still need a workaround: you can select every second hole with the Centerline command and it will work...

[GG_Dynatec]

Thanks for your help. That explains why the circles come as arcs in the views of the machined faces. Also, your suggestion gave me an idea to make the tool do what I wanted for preserving the integrity of the annotations when selecting a different state of the model. 

What I can do in one step on the non-machined side of the flange with the "Centered Pattern" version of the tool, I have to do in 3 steps on the opposite side. First, I use the "Centerline" from the hole at 0°to the hole at 180°, then repeat from the holes at 90° and 270°, then use the same tools in the remaining holes. That gets me as close as possible to where I need to because all the flanges in that family size have the same number of holes. I just made a quick test on 10" flanges that have 12 holes as opposed to 8 and discovered I would need to re-draw in 4 steps every 60°instead of 3 steps every 90°. 

Thanks for your help. 

[johnsonshiue · Accepted solution]

Hi! Many thanks for sharing the files and findings! The main reason why is behaves this way is that the edges are intersection edges (3D spline curves). These edges are projected back to the view plane. They look circular but they are not true circles. As a result, certain workflows targeting true circles may not work properly.

I need to work with the project team to understand it better. However, I don't anticipate a quick fix.

FYI, this has been reported as INVGEN-63089.

Many thanks!