Position Representations in Weldments not allowed?

[Dustin Green]

Does Inventor 10 not allow position representations to be created in Weldments? I Right Mouse Button (RMB) click on "Position" under "Representations", but "New" is grayed out.

[Anonymous]

Dustin,

Positional representations cannot be made in a weldment assembly; however,
you can create the weldment (the rigid part) and then place it along with
the other components that you would like to participate in the mechanism in
a higher level assembly. You can then model the mechanistic behavior in that
assembly.

Regards,
Joe Doyle

wrote in message news:4979027@discussion.autodesk.com...
Does Inventor 10 not allow position representations to be created in
Weldments? I Right Mouse Button (RMB) click on "Position" under
"Representations", but "New" is grayed out.

[RUBE]

Has this been fixed yet. Why is autodesk limiting the use of the software. i need pos reps in weldments.

[Josh_Petitt]

I think the rational was that a welded assembly does not move relative to any of the other parts. If you need to change the position, then break the weldment into two (or more) weldments and then combine in an assembly.

[billco-mfg]

The request sounds like it doesn't make sense, but I know I've wanted the same thing in the past. I just don't remember why.

[RUBE]

Say you have railings with a hinged gate. The hinge is welded to the gate and the rail. There is no way to show the gate in the open and closed position in the weldment. (do not want to make it adaptive or have two hinges in different positions inside the weldment and use design views.) Also what if you have a fixture that uses clamps. The clamps are welded to the fixture and have different positions. would be easier to use a positional rep to show the positions.

[Josh_Petitt]

>Say you have railings with a hinged gate.

you have a weldment with gate welded to one side of hinge and a weldment with rail welded to other side of hinge. Put both weldments in a sub-assembly and use hinge for constraints.

[RUBE]

You are not getting it. The hinge has welds to the rail and the gate. Thus it is in the weld enviroment.

[R.Corriveau]

Isn't the rail and gate actually two seperate pieces joined by a hinge?

So why not weld one half of the hinge to the gate (gate weldment), weld the other half of the hinge to the rail (rail weldment) then mate them together in an new assembly about the hinge?

[Allen_Gager]

My hinge is a single purchased part that is already joined. I'd like to show it as such without needing to go thru extra hoops to get there. Nor should we have to create extra models and processes when it could be done with a PosRep. As you suggest it would create two weldments, plus another assembly.

-AllenG

[cvbt-thailand]

My use for positional representation in a welded assembly is to try different positions for an idler pulley pivot that is welded on a frame.  My work-around will be to do two view representation with two pulley pivots.

[dwweekly]

I have the same frustrative difficulty.

I have a Destaco clamp that has positions
and I need to weld an extension arm on.

This is quite common. In many tooling shops.

I initially download the step file of the manual clamp
then constrain it.
Make up my positions
(usually - free , open, closed)

I insert this clamp into my weldment

Then if the weldment template would work .....like an assembly.....
I would then select the positional represtentaions of the clamp
and add them to the postional representations of the new file (the weldment assembly)

add my ipts that I am to weld on to the clamp and the place the entire weldment into my main assembly
and be able to actuate from the top assembly level

oh well , current workaround
I use an assembly template instead and dont show weld on the detail
The build shop will just has to assume
or I will just flag out some "weld here" leaders.....
oh well.

[JDMather]

I would do the Position Repswith the sub assembly.  Seems to me like it would be more representative of the real world.

[will3X6V4]

To my knowledge this still hasn't been addressed.

There are many cases where subassemblies that have moving parts must be welded together.  The final assembly inherits the same movement as the subassemblies.

It does not make sense to "break" a subassembly apart, in order to bring it back together at a later stage.

It also doesn't accurately reflect manufacturing sequence.  If I have a captive part that is free to move, but restrained by a welded part (retaining pin, stopper, etc.), the moving part must be placed prior to welding the part that renders it captive.  By inserting the moving part at a later point in the hierarchy, it will be incorrectly placed in the BOM.

Similar to the hinge example above - if half of the hinge is part of assembly A, and half is part of assembly B, then you will have two separate items in the BOM, shown being welded in separate steps as part of separate subassemblies, when in reality you complete subassembly A, you complete subassembly B, and then you weld A and B each to a single hinge in one step.

While I understand that a welded unit cannot move within its welded connections, and I'm sure that was the idea behind this limit, there still needs to be a function that allows for unrestrained parts to move, and be represented in multiple positions.  The software should always endeavour to facilitate and communicate the same processes and results available in real-world fabrication.  I shouldn't be forced to show my drawings as Step 1, 3, 4, 2.  I should be able to show my steps in sequence the way I expect the fabricator to do the work.

Does anyone have any updates or anything to add to this issue?

[jaskiratVPK8U]

If position representations are not allowed in weldment that how can we create welding assembly instructions? I need to show before and after welding isometric views. Why there is always a work around in inventor instead of having straight forward solutions.

[swalton]

Position reps are different than Design View reps.  Weldments allow Design View reps, which I use to define each step for my complex weldments.  One limitation is that 3d weld beads are treated as a single body.  That means that I have to show all 33 beads or none of the 33 beads in my weldment.  I could not show only the beads attached to the visible components in each weld step.  

I have started using cosmetic welds and Design View reps to build welding assembly step drawings.  That eliminates the all-or-nothing issue of the 3d beads, but brings up another issue.  I was not able to find a way to show the weld symbols by step.  Instead, I had to show all the symbols, then delete the ones that did not apply to the specific view.  I added a Step Number count to the note field in each weld symbol.  That way I could quickly pare down the 33 symbol for the entire weldment to the 3-5 symbols necessary for an individual step.  

I do not believe that Autodesk expected anyone to use the combination of Design View reps, 3d or cosmetic weld beads in the model, and Get Welding Symbols to retrieve the Model Weld Symbols on 2d drawings.  This seems like an obvious way to document complex weldment instructions, but the current workflow is bad.

[johnsonshiue]

Hi Folks,

Indeed, Positional Rep is not allowed in Weldment. It is because Positional Rep only deals with component position, which does not involve shape change. Similarly adaptive does not work with Positional Rep either.

I think what you are asking is related to the Model States project we are working on. If you are interested, you can sign up Inventor Feedback Community (https://autode.sk/InventorBeta). You can try it on a browser-based install-free environment. The project teams are eager to hear your feedback.

In the meantime, on Inventor 2021 or earlier, you will need to use iAssembly (multiple members) or iLogic (multiple iam files) to show welding steps.

Many thanks!

[jaskiratVPK8U]

I am new to inventor, I used solidworks before, it had option to create exploded views of assembly and those can be used to show different welding stages for a weldment assembly. I think I can only use view representations to show welding steps inventor. 

[Marco_mendez]

I think your Assembly is not on Standar must be on Weldment or Mold. (Can't create New position on it)

[johnsonshiue]

Hi! To clarify the issue, the original discussion was about not being able to create Positional Rep in Weldment assembly. This is indeed a limitation. Positional Rep is limited to only change in position. Change in shape is not allowed. Depending on the Weldment state, assembly geometry can be different.

The requirement of showing positional difference and geometric difference within a Weldment assembly has been fulfilled by Model States in 2022 (Pos Rep remains position only).

Regarding the automatic Exploded View support in Presentation environment, it is unfortunately discontinued. You will need to tweak individual components to a new place in ipn.

Many thanks!