Losing *hours* of productivity due to serious Frame Generator bug (Inv. 2015)

[RobertWK]

So I'm having quite a serious, frustrating problem that is setting my project back probably about a day or two every time I have this bug.

The workflow pretty much goes like this:

1. I'm inserting a frame member into an assembly using the frame generator.

2. I place the frame member where and what rotation it needs to be in, and then trim the frame to the faces in order to make it the length it has to be.

3. I'm choosing "Reuse" in order to reduce the amount of files that ultimately are uploaded to vault.

4. I select two or three other lines which are supposed to have the identically sized and oriented frame member.

5. I do apply, and the frames are on the correct line, however they are rotated incorrectly and they are somehow offset from the position they're supposed to be in. 

6. At this point I do a "Change/Reuse" and rotate or mirror the frame, and because I figure it's running the wrong way, I do a 'flip member direction'.

7. Unfortunately at this point when do I an apply, I get either one of two results. The first is that everything works OK. The second is that now the frame is completely on the other side of the fence and it's also oriented incorrectly. Additionally, now some OTHER member that I have done a REUSE on is now also incorrect.

8. To fix it, I decide to do the same steps on the other frame member, which may or may not work correctly.

9. Unfortunately, it doesn't work so I delete the reuse, which causes yet ANOTHER member to reorient itself incorrectly.

This tends to go into a maddening cycle.  I took 11 screencaptures to show what is going on, but I would rather send them directly instead of posting them here (Don't want to spam the board).

If anyone, anyone can help or if there can be a hotfix for this I would be so incredibly appreciative.

[RobertWK]

Except I think copy/paste adds another file to the assembly, whereas reuse does not and thus reduces the overall size of the vault. Just because the tool isn't working doesn't mean it shouldn't be fixed.

[jtylerbc]

That might be viable as a temporary workaround to meet an immediate deadline.  But the Reuse feature was introduced largely to eliminate these sorts of extra steps and workarounds.  It needs to be fixed.

[wimann]

Oh well yeah I completely agree, the tool ought to work and if it doesn't, it definitely needs to be addressed. While I agree with that, I'm not as certain that copy/paste will add any more than using the Reuse tool would. But, again, I don't use the Reuse tool. Does it display the member without adding a part to the assembly? I had imagined that it just places another occurance of the selected piece in the orientation you specify (bugs aside). Which is essentially taking the few steps of selecting the .ipt, pressing ctrl + C, V, and constraining and combines them into one tool.

Anyway, maybe someone else will have more insight on that particular tool. All I'm saying is that if the tool is malfunctioning, it's great to flag it and inquire about it but for the time being, alternate routes may be the way to go. Seems like that tool is new to inventor (since I'm in 2014 and don't have it) so it's no shocker that it's buggy.

Wish I could be more help.

Thanks,

[wimann]

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@jtylerbc wrote:

That might be viable as a temporary workaround to meet an immediate deadline.  But the Reuse feature was introduced largely to eliminate these sorts of extra steps and workarounds.  It needs to be fixed.

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Couldn't agree more.

[jtylerbc]

wimann,

Reuse is a 2015 feature, so you are correct, you don't have it yet.  As for what it does, your interpretation is pretty much dead-on.  RobertWK is mistaken in thinking that your Copy/Paste solution adds an additional part to the assembly - it would add another instance of an existing part, which is what Reuse does as well.  From a file management perspective the two solutions are identical.

[RobertWK]

My apologies; I thought that it created another instance of the geometry as a file.

[ajcraig99]

Yo Johnson!

Thaught you said you were on holidays....

Still having a very simular issue to this in IV 2014, except without the 're-use' feature obviosly.

when you get back from holidays can we resume the whole tech support thing in regards to this??

[johnsonshiue]

Hi! I was on a business trip and I was not on holidays. I was able to check the board occassionally. I am looking at this issue now.

Thanks for your patience!

[jtylerbc]

See attached for another example of a frame with the problem.  The reused instance of the orange tubes will reverse direction if any change is made to the layout part.

It doesn't even have to be an actual geometric change - if you just open the layout part, Rebuild it, then update the assembly, the orange tube will reverse direction.

The model is so insistent about reversing the direction that it will even defy constraints to do so.  On another copy of this model (which I did not keep), I attempted adding constraints to keep the ends of the problem "Reused" tube flush with the original.  As soon as I made a change to the layout, the tube reversed directions and the constraints I had added were rendered Inconsistent.

[dano0310]

Just wanted to bump this to the top again.

[shandavis316]

Ill help you bump 🙂 im reading this thread and there are some questions in my mind that need more answer. i'll follow this thread.


cheers
shan

[karirafn85]

Another bump.

The "Reverse member direction" option of the Change Reuse dialog is reset every time the frame is edited (or the rebuild all operation is called).

I've attached an image that I feel does a good job of explaining the problem in a simple manner.

[smokes2998]

Hi does the 2016 version frame generator auto reuse members based on length and type of cuts yet?

The competitor software that I have used extensivly does this and does not generates a part file for each

member.

The frame members are stored as virtual sweeps with in the assembly or model file depending on which CAD software I use, which makes it a lot easier check into the vault. This would make my life easier for pipes as well.

[jtylerbc]

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@smokes2998 wrote:

Hi does the 2016 version frame generator auto reuse members based on length and type of cuts yet?

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No.  The "Reuse" feature being discussed here is not an automatic reuse.  It is a manual way of telling Inventor to reuse frame members (which, obviously from this discussion, still has some quirks.)

[smokes2998]

So its still quicker and more stable to manually extrude/sweep frame parts and  mate them in an assembly than use than frame tool still. grrr. Why create such an unproductive tool....

Every other frame tool I have used it a case of draw a 3d sketch in a assembly in the case of SE  or  the part file in the case of SW populate the sketch with profiles trim the profile add features and other welded parts add welds and hey presto you have a cut list. And the ablity to detail the unique feature of the members. it did not create a new part for each member and this made it easier when you had to change profiles and check it into the vault. 

[jtylerbc]

It's not perfect (this thread is evidence of that), but I definitely don't agree that it's more efficient to make your own parts.

For the most part, it does everything you list.  You make a "skeleton" part to lay out your frame, and then select the profile you want to apply to it.  Where it differs from what you describe is that it creates a part file for that member, rather than making it some sort of "virtual" (not sure of the proper terminology here) part in the assembly.  These parts show up in a normal drawing parts list, so getting a cut list isn't really a problem.

With the Reuse Member feature (which was new in Inv. 2015), you can reuse identical frame members rather than generating duplicate part files.  The weakness of it is that the system doesn't recognize the duplicate members - you have to recognize them yourself.

It is still far better than manually making your own parts in most cases.  If you want to have frame members automatically trimming off to each other as the design is changed, without using Frame Generator, it would require a ton of adaptivity.  That would certainly be unstable.  The only advantage to making your own parts is the reduction of files - you pay for it in every other respect.  And even then, you're manually reusing the files, so all you've done is take the long way around to making your own "Reuse Member" feature.

I realize you've used other software that operated differently.  It may have even just been hands-down better at frame design than Inventor.  But I have yet to see another method in Inventor that does a better job at it than Frame Generator does.  If you avoid using the best tool you have for the job now because it's not as good as the tool you used to have, you're just hurting your own cause.

I'm sure you'd find plenty of people here (myself included) willing to help if you have questions about how to deal with Inventor's Frame Generator and make it work for you.

[wimann]

Yeah I use FG all the time and have no real issues with it.

But I've already chimed in once in this thread (hence why I'm following it). Seems like an echo chamber at this point.

Nope. The software doesn't do everything. All you can do is post the features you would like to see in the idea station and cross your fingers. Other than that, you gotta work with what you've got.

[smokes2998]

It does bug me me a lot that the 3d sketcher is no where as good a it competitors and having to create a skeleton.ipt to get around the lack of a decent 3d sketcher in the assembly is stupid. The biggest problems with FG is that it can generate a lot of members and if you end up deleting and editing memeber profiles and if you check the frame in ever night you end up with a lot extraneous parts in vault. It is especially bad from a time sap point of view when checking stuff in and managing parts in a global vault with 65K + plus files and having to sort out the member file names so that they don't conflict with other files in the vault. Please note frame members in my case don't usually have part numbers typically they are cut to length before manufacture so are considered raw stock.

[RobertWK]

I have found that a somewhat permanent workaround is to only use "point" selection in order to place the frame members, and almost never to use "line" selection under any circumstances.

Using "point" or "end to end" selection seems to allow you to choose direction and limits by the order in which you select your endpoints. Selecting the line is... I guess arbitrary?

I feel like it stinks just to limit yourself to one function, but there you have it..

[jtylerbc]

In my experience, it's not technically arbitrary, but it can certainly feel like it is, especially if there is a significant gap in time between when you originally placed the member and when you try to Reuse it.

It has to do with the combination of which end of the line you picked closer to when you placed the original member, and which end you picked closer to when you placed the Reused member.  This would not be a serious problem if the member direction flip option worked properly, but it doesn't (which you already know, as it's part of your original problem that started the thread).