Inventor Assembly Cannot Create New Position View Representation

[lkirit2000]

Hi 

I do trestle assy, I am in a stage to show fully extended and fully closed position. So In the model tree I right click to make a position, but there is no option to as NEW to create positons. 

How to fix, please ?

kelly.young has edited your subject line for clarity: New Position - Assy File

[Mark.Lancaster]

@lkirit2000

Inventor version?  Perhaps show a screen shot of what you're seeing.  Make sure to include browser info as well.

[MSD_takaseh]

Hi lkirit2000,

I think the issue you are facing is data specific.
Here is a general diagnostics but please try the followings if fix the issue.

1. Open the assembly file and Rebuild All.

2. Close Inventor once and Reset Inventor setting with the reset utility from here.

3. Remove a content of %temp% folder. (There might be unremoved file in there)

4. Run the Inventor as Administrator with RMB.

5. Set User Account Control of Windows to "Never Notify". (Reboot the machine)

6. If you don't yet apply the latest service pack/update then please apply.

Thanks.

[dgreatice]

Hi,

to clarify:

where you right click? Browser(Model) > Representations > Position? or else?

Or you in Assembly Weldment Mode ? if yes, you cant make Positional representation.

[johnsonshiue]

Hi! You probably are in Express mode. Click on Load Full so the assembly is fully loaded and all workflows will be available. If it does not work, please attach a screenshot.

Many thanks!

[christophe.moerman.external]

Hi,

Or you in Assembly Weldment Mode ? if yes, you cant make Positional representation.

why can't? Suppose I have two options with sizes A and B so the welder must use A or B according to the order.

best regards,

Christophe

[SBix26]

Sounds like a good application for Model States.

Can you attach an example assembly and describe what you're trying to accomplish?

---

Sam B

Inventor Pro 2023.2 | Windows 10 Home 21H2

[christophe.moerman.external]

it is steel pallet for forklift truck. Two rectangle profiles have variable dimensions A. eg. A= 500 or A= 800 etc... It is for the welder to place the rectangular profiles at the correct distance according to the order. So "weld assy" doesn't work. only with plain assy.

[johnsonshiue]

Hi Christophe,

Sam is right. PosReps are not available in a weldment assembly, because a PosRep does not allow the geometry to change. Model States are the way to deal with the request (except enabling Flexible status). As PosReps, Model States also supports Overlay views.

Many thanks!

[jtylerbc]

Before Model States, I think this still would have been achievable using iAssemblies.

Using Positional Representations for something like this pallet is a misunderstanding of the logic behind them, in my opinion.  PosReps are for situations where an assembly can move.  Think of something like a hydraulic cylinder - when you extend or retract it, that isn't a design change.

For the pallet, you're really talking about design variants.  No individual pallet will ever have two different spacings of the fork tubes and be able to switch between them.  Instead, you're making "A" and "B" variants of the design.  iAssemblies or Model States are both more appropriate tools to use in that case.

There are cases I have seen where PosReps in a weldment would be completely logical.  I tried to find an example of where we have done this at my company previously, but had no luck, so I'll just have to describe it.  Imagine a tube welded to a larger piece.  A lifting link is installed on this tube, but is not welded (it pivots around the tube).  A capture plate is then welded to the tube.  Thus you end up with a piece that can move, but is retained by a welded piece.  Inventor does not handle this scenario very well.  If you make the assembly a weldment, you can't move the link (no PosReps or Flexibility).  If you don't make it a weldment, you can't show the welds.

In short, I think there are good reasons to have PosReps available for weldments, but the pallet example here, in my opinion, isn't one of them.  Existing tools (iAssemblies and Model States) already do a better job of reflecting the intent with that application.  But there are definitely situations in the real world where assemblies that are welded together still have some movable (but not removable) parts.

[johnsonshiue]

Hi John,

Strictly speaking, it is yes and no. iAssembly may be able to show an assembly in different positions. However, Overlay view does not support iAssembly. Nor would it allow change in geometry. Plus, the flexible status isn't configurable either.

Many thanks!

[christophe.moerman.external]

My motto is keep it simple. I prefer simple configuration and never use iassembly. Too bad iassembly doesn't support welding.
Because I can't convert weld assy back to plain assy.... That's exactly why I have a problem with position....
I close here. Because it's an absolute waste of time. A small drawing takes fifteen minutes. Finding a solution takes 1 hour....

[jtylerbc]

---

@johnsonshiue wrote:

Hi John,

Strictly speaking, it is yes and no. iAssembly may be able to show an assembly in different positions. However, Overlay view does not support iAssembly. Nor would it allow change in geometry. Plus, the flexible status isn't configurable either.

Many thanks!

---

All of that is true, but doesn't really come into play in the pallet example.  There you're really modelling two different static real-world assemblies (not a single movable one).  It's unlikely that you would ever need to Overlay two different pallets on top of each other, and they don't need to be flexible because nothing actually moves.

So these are limitations, but often wouldn't actually be a practical problem.  I've used iAssemblies before to model related weldments (usually left/right hand versions), and it works well for static weldments.  So it would be a solution for the pallet, but it is not a solution for the "captured link" example I gave (where a piece is actually movable in the real world).

[jtylerbc]

---

@christophe.moerman.external wrote:
Too bad iassembly doesn't support welding.

---

Yes, it does.  I just created an example file doing exactly that (see images below).  A main plate with lugs on the side, and three configuration options:

1. Double Lug
2. Right Lug Only
3. Left Lug Only

The iAssembly table includes columns for Include/Exclude for the lug parts and their associated welds.  If there are parts (and welds) that appear in all configurations, they don't need to be added to the table.

Note:  Your pallet assembly could be handled this same way by having two copies of the upper tubes, and Including/Excluding them as needed.  However, a better method would be to have just one copy of the tubes, and change the value of the constraint offset that positions them (similar to a PosRep).  When set up that way, your pallet is actually a simpler iAssembly than my example.

Double LugRight LugLeft Lug

Browser

iAssembly Table

[christophe.moerman.external]

Dear 

@jtylerbc

I added now Iassy (A=270 and B=450). It works. Thanks but,

How can I update the drawing? It is not correct and strange. see second picture

regards.

[jtylerbc]

Edit the view and look at the "Model State" tab.  In the dropdown list at the top, you can set which iAssembly member is active in the view.  If you created the view before converting the assembly to an iAssembly, it may be confused about which member to use until you set it, and thus giving weird results.

If not that, then how are those values being created on the drawing?  Is one of them manually typed?  If they're both parameters, are you sure they're using the same parameter?

What is the thickness of the tube?  Could your constraints have been accidentally set to the inside wall instead of the outside?  Could explain the difference if the tube thickness is 10 mm.

I threw out a few ideas for you to check, but this issue may be a little tough to troubleshoot without seeing a copy of the files.  I'm still running Inventor 2021, so even if you posted them I wouldn't be able to check it out if you're on a newer version than that.  Others would though, so if you don't mind posting the files that's probably your quickest route to a fix.

[traviscwright]

Thanks for your insight and help. I was indeed looking for the design variants. But, I'm not quite sure about your answer. Could you please tell me if the following scenario would not require a PosRep? Let's say you have a hydraulic cylinder and in the design you have different dimensions of the cylinder. The base of the assembly will have a certain dimensions and the top of the cylinder will have a different dimensions, so that one can move to the other. The cylinder in this case will be inserted in a certain pose and the top of the cylinder will have the dimension that allows it to move to the other pose. So, if I understand you correctly, in this case, there will not be any design variant involved and hence, the PosReps are not required? Thanks, again.

[christophe.moerman.external]

Exiting inventor and restarting solved the problem.