Flexible assembly issues

[Anonymous]

Hello,

I have a piping assembly in inventor. This piping is divided into two separate sections (I don't use the piping tool because it wouldn't be applicable for this type) with a coupling in between. The first section is set with a 2 degree slope (first picture). this couples to a different section that is at a 2 degree slope until the end where it becomes parallell to ground (Second picture). I have assigned constraints on the parts with a max/min distance of +10,000/-10,000 so they are flexible and assigned no angle to it. These two combine in an assembly with the second section as flexible so that I can adjust the pipe lengths as necessary. 

Section 1Section 2

The square flange will be attached to an object and the end piece on a different object. I've tried it using a single assembly where it worked, but with these two separate assemblies it doesn't want to work. When I attach the flanges to their respective parts, it wants to sit like following:

However, I don't want the second section to be angled like that, I want them to be parallell. When attempted, this fails though. 

Due to confidentiality I cannot provide the assembly files, I'm sorry to say. but I can provide any other information that may be necessary.

[mcgyvr]

Without seeing the specific constraints,etc... applied its just guessing and we really don't have much to base our guesses off of.. 

If you don't figure it out I suspect an Autodesk employee will come by eventually.. You could share the dataset with them with an NDA

There are some "known problems" with the constraint solver and flexible assemblies though.. I suspect you have just stumbled upon one..

If designed to be correct at 2deg why not remove the min/max and enforce the 2deg and see what happens..

Good luck..

[Anonymous]

Hi,

I can't remove the min/max constraints, because I only have vague ideas about the distances necessary, and they aren't integers and Inventor requires 100% correct numbers to mate correctly. I do need the concentricity of the different parts in the piping sections and I can either use concentric constraint or insert with max/min and the result should be almost equal. I have tried forcing the 2 degree angle and the result doesn't change. The problem is still there. It's no problem showing the sections by themselves, only the surrounding areas that the sections attach to, so I can provide the mates I have used. I don't know the best way for this though. I don't wish to pack&go because it would contain all the information we have in our template. 

The assemblies are almost completely made from content center parts, except the square flange, which is our design.

[johnsonshiue]

Hi! In some cases, the angular limits may not be enforced because it could drastically reduce the degree of freedom. Please share the files (iam, ipt) here so forum experts can take a look.

Many thanks!

[Anonymous]

Hello, I've compiled the parts and the assembly for section 2 in a zip file. I hope this will suffice as an example. 

I can provide section 1 if needed, but I'll remove the square flange if that's the case, but there are no issues with section 1. 

[johnsonshiue]

Hi Adam,

Many thanks for sharing the files! I took a look. I am still trying to understand your request. Is it about not being able to rotate "DIN 2982 R-208 Welding nipple ISO Taper:1" 90 deg? If yes, it may have something to do with Angle:2. It prevents rotation from happening.

Could you elaborate what exactly you were looking for?

Many thanks!

[Anonymous]

Hi,

Angle 2 is there to ensure that the section is constrained parallel to to the XY plane and thus not able to rotate on the axis of the flange. Together with Flush: 2 and Mate: 2, this ensures the angle of the welding nipple. I found this way to be the easiest way, but maybe it's not the most proper way.

The issue is that when I constrain it to section 1 and to another part further away, it get stuck in an angle, as demonstrated in the original post, and I cannot change the angle of it, which should be possible due to insert: 2, Insert 3, and Insert:10 being as flexible as they are. The constraining to section 1 and the second part is only an insert constrain, without any angular constraint. When i try adding an angle 0° to a plane I want section 2 to be parallel to, it fails.

[johnsonshiue]

Hi Adam,

I think I know the behavior you are talking about. It could be a bug or just the way it works. But, I need to see the exact failure in order to comment further. Please share the entire assembly including Section 1, so I can reproduce the failure.

Many thanks!

[Anonymous]

I stripped it down to just the sections with section 1 grounded and the other side replaced by a grounded loose flange. The error persists so it should be good for checking.

Thanks

[johnsonshiue]

Hi Adam,

Many thanks for sharing the files! I see the issue now. I think this has something to do with grounded components. There are two places in the assembly with excessive grounding. 1) DIN EN 1092-1 TYPE 02 Loose flange PN 10 1.4307-15:1 at the top level is actually grounded. Right-click on it and uncheck Ground. 2) Within Section 2, the first component is also ground. Uncheck Ground.

After that, the assembly should work desirably. Could you try it and see if you are seeing the same behavior?

Thanks again!

[Anonymous]

Hi,

Thanks for looking into the assembly. Responding to your 2 points below:

1) The loose flange that you are referring to is a placeholder for a part that isn't to be moved. I can't unground it because it would lose it's purpose as a placeholder. Obviously if I remove this grounding, the assembly would find a way, but the flange would also move, which I can't allow.

2) I need a grounding in section 2 so that the assembly has defined planes in logical places. I did try to remove the grounding on it just to test it though and it doesn't solve the issue.

[johnsonshiue]

Hi Adam,

Many thanks for the explanations! They do make sense to me. But, what about Angle:1 at the top-level? It seems to conflict with how the components are constrained. Is the angular constraint needed?

Thanks again!

[Anonymous]

Hi,

What I want is for "Seamless pipe 21,3 x 1,6 - 544:1" in Section 2.iam to be in the same YZ plane as "Seamless pipe 21,3 x 1,6 - 200:1" in Section 1.iam. Angle:1 in Main assembly.iam is there to make sure they are in the same YZ plane as each other.

[johnsonshiue]

Hi Adam,

I think there are conflicting constraints. Here is the proof. Suppress Angle:1 at the top-level. Then measure the angle between the two supposedly parallel directions. You will there is a small angle. Either you need to change the geometry or change the way the components are constrained.

Many thanks!

[swalton]

@johnsonshiue Does the Explicit Reference Vector angle constraint option solve better than the Directed Angle option in flexible assemblies?

@Anonymous Why isn't DIN EN 1092-1 Type 02 Loose Flange PN 10 1.4307-15:1 orthogonal to the origin planes of Section 1:1?  As I open the Main Assembly file, it sits at an angle to Section 1:1.  

If I constraint that flange with explicit offsets from Section 1.iam, then I can enable Mate:49 and Insert :86 in the main assembly.  

[Anonymous]

@johnsonshiue I am aware that it seeks that angle. I mentioned it in the OP. However, by all logic, it should be able to sit straight rather than at an angle. 

@swalton Thanks for checking. I didn't notice the angle. That was a mistake. However, upon fixing it, the errors persist. You say you manage to get it working this way, could you attach the assembly file for me? Thanks in advance

[Anonymous]

I need to bump this just in case you missed my reply, @swalton . Could you send the files concerning how you fixed the issue? Many thanks in advance.

[MoshiurRashid]

Create a referance plane and make a constrain (angular) with the midplane with that cylinder.

[swalton]

@Anonymous 

Here is my solution in Inventor 2019 format.  I had to do a bit more to get a full solution

I cleaned up the extra constraints in the Section 2 Assembly that made it hard for the constraint solver to resolve.  I also made sure that the insert constraints flowed from the grounded component to the final straight fitting.  

[Anonymous]

Hi,

Thank you very much. However, I use Inventor 2018. If it wouldn't be too much trouble, could you convert? It would be appreciated greatly. Sorry for being a bother here.