Rectangular Pattern tool question. Bug or a feature?

[Ivan_Sinicyn]

Me again😉

Now I'm interested in the operation of the rectangular pattern tool.

If you make a pattern along the length of the curve in one direction, then everything seems to be fine, but as soon as you turn on the direction of symmetry, the result becomes completely unpredictable. The length of the curve becomes 2 times longer, in the preview the number of objects is 2 times less, and the result is generally amazing.

[JDMather]

When creating a curve driven pattern dividing the Curve Length - go in only one direction.

I cannot think of a logical reason for attempting Midplane?

[Ivan_Sinicyn]

For example, when the part has a more complex shape and the contour of the pattern is not closed.

[JDMather]

You did not Attach the new file here?

You have to tell Inventor what you want.

If you want the path open - then use open path (and consider Start position).

If you want closed path - then use a closed path.

Your Design Intent is not clear to me.

If it is not clear to me - then it is certainly not clear to the software.

Can you elaborate on your true Design Intent (perhaps a picture of something similar from the real world).

Can you Attach your file here?

[Ivan_Sinicyn]

My experience in the Inventory is about 7 years. I have no problem solving this problem. It's pretty simple. I'm just sharing my experience, which tells me that this is a bug. I haven't found a section for bugs, so I'm writing to the main one. I see there are software testers on this forum who can discuss this with the development team. I want to contribute to the development of the product so that it gets better and better with future releases.

But back to the Part. The preview of the task being performed shows that I have chosen the right strategy, but the result is different. Interestingly, if the pattern creates each body separately, then the operation goes correctly.

I have attached a new file.

[IgorMir]

Hi Ivan,

I really have a hard time to reproduce what you are describing. Yes, it can be reproduced but only if the selection of parameters in the Rectangular Pattern DB is going in a wrong way. Here are two quick files in IV 2020 format. In Part1 I have done my best to ruin it (un-dimensioned sketches and so on) - but the pattern still works as I would have expected it to work.

That's all I can say about it for now.

Cheers,

Igor.

[Ivan_Sinicyn]

Hi Igor!

This task does not require any cutouts. The task is to make one body flow around another body along a contour or along a limited curve. You need to switch to working with bodies, not elements. Also, it is not known in which version of Inventor this bug appeared. I am running version 2023.0.1

I've been working with your file.

In fact, you don't even need the first body. It is enough just to make a body pattern along a curve.

[IgorMir]

Hi Ivan,

Such an outcome can be if the pattern's start point is not specified. Otherwise - I got no problem with it. At least - not in IV2020.
cheers,

Igor.

[Ivan_Sinicyn]

And again. You are working with element patterns, not bodies. In the process of developing a part, you can perform a dozen operations and you will have to make a body pattern, not each element. I'm just giving a simple example of how to reproduce the problem.

[IgorMir]

Beats me what's going on at your end. Here is a file in which I was trying to mimic your design. I got zero problems creating the part. Maybe it is something in a newer release. But I leave it for other people (with access to a newer version of Inventor) either to confirm or dismiss it. Since on my end - I am not able to reproduce the error you are claiming there is in the latest Inventor version.
P.S. From a screen shot of yours you are selecting "Идентично" option in the right hand side of Rectangular Pattern DB. Try to select "Направление 1" instead. 

PPS - I was trying to swap the selection between "Идентично" and "Направление 1" in the sample I have posted. And even tried to create a new Pattern using the exact settings of yours. Still - I got no faults. With either of the settings I get the identical result to what I have attached in here.

[Ivan_Sinicyn]

You are modeling the sequence incorrectly. You need to make a pattern - The whole part, not a separate element!

This is what happens when you select "Direction 1" (Направление 1)

[IgorMir]

I see...
But with all honesty - it didn't cross my mind to use Pattern Solid option in your example. By doing so - you include the pass into the pattern as well. Yes, by doing so Inventor is getting confused. The definition of what is the pass and what is actually the body you want to pattern is getting mixed up. Yet if you chose the "Pattern Individual features" instead - it all works as expected.
The same applies to the previous samples I have posted. If you want to get the round object patterned along the edge of a rectangular object - you should keep the rectangular object out of the pattern set. But if you want to pattern the whole solid - and auxiliary sketch got to be created. Geometry of which will be used as guidance for the  pattern.

[Ivan_Sinicyn]

Before proceeding with the patern, you can perform many operations with the body. Moreover, the construction process can be so complicated that you simply won't be able to select all the elements to build a template. There is an option for this - a solid body. This option simplifies the calculation process for the program several times. I don't understand what the program can get confused about there. This is the same operation performed on the same curve, but with a solid body, instead of its individual elements. And yes, in the previous examples I also used an auxiliary sketch with an auxiliary curve. The result is the same.

Well, as I said, if you enable the option to create each copied object as a new body, the problem disappears.

The problem most likely lies in the incorrect assignment of the ID for the elements, which is why one of the elements of the pattern takes the starting position instead of the base one.

[SBix26]

I can easily reproduce your results in 2023 on my computer.  This must be a bug, since it works as expected when creating a feature pattern or a pattern of individual solid bodies.

The obvious workaround, I guess, is to create individual solid bodies and then Combine bodies to create just one.

Question: why do you want one solid body consisting of dozens or hundreds of separate lumps?  Why not create dozens/hundreds of bodies?

Update: the same occurs in Inventor 2020.  See attached file.

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Sam B

Inventor Pro 2023.0.1 | Windows 10 Home 21H2

[Ivan_Sinicyn]

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@SBix26 wrote:

The obvious workaround, I guess, is to create individual solid bodies and then Combine bodies to create just one.

Yes, that's why I ❤️ Inventor. You have the opportunity to solve the problem with different tools.

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@SBix26 wrote:

Question: why do you want one solid body consisting of dozens or hundreds of separate lumps?  Why not create dozens/hundreds of bodies?

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There are different ways of modeling. Yes, in the current situation, you can create a bunch of new bodies and merge them, but I created the topic so that testers or developers would pay attention to the bug.
I have been working in this "working environment" for many years and I care about the future of the program. I want to contribute to the quality of work.

P.S. And I'm sorry if I'm not explaining things well enough. I'm only learning English and have to use a translator.

[johnsonshiue · Accepted solution]

Hi Folks,

There is no argument this is a bug. It should just work the way as in the preview. Indeed, keeping each body as a separate body seems to make it work, which again proves something is wrong with the Join option.

This is a great catch! It has been reported as INVGEN-61899. I will work with the project team to understand the behavior better.

Many thanks!

[Ivan_Sinicyn]

@johnsonshiue 

The bug was fixed in version 2023.2, but it seems that part of the source code was taken for the new axis pattern function.

Here is an example:

The preview shows correctly, but the result is different.

[BDCollett]

It's great to point out these bugs. Sure, there is always a workaround, that is beside the point. 

If they are not tested by someone and brought to the attention of the developers, then they will never get fixed.

[johnsonshiue]

Hi Folks,

We remain imperfect. The fix to INVGEN-61899 in 2023.2 introduces yet another regression as Ivan pointed out. We are backing out the fix in the coming 2023.2.x update. The proper fix cannot be ported to existing releases. Only the new release can have the fix unfortunately. We are sort of back to square one at the moment.

Many thanks!

[frederic.vandenplas]

Same here