Frame does not change when sketch is changed

[n00kie.tdc]

Hey fellow Autodesk users!

Faced such an issue:

I am building frame using frame generator. Well, firstly I build a sketch and then afterwards from that sketch I already make frame itself.

What I want to do iis when I am changing length of some frame memebers in a sketch, I want frame members to be changed as well.

For example:

From here you see that everything is ok. Frame members are according to the sketch.

But when I am changing the sketch, frame stais as it is on the first picture without any changes. Previously it was changing, but then something happened and it doesn't change anymore.

Can anybody explain me what am i doing wrong? Could it be some representations issue? Or is it something else?

For me it seems that reference skeleton of a frame is not referenced to the sketch of the frame .ipt. 

Thank you for explaining and taking your time for this.

Regards,

Vadim. 

[Anonymous]

Buenas tardes en este link se encuentra la solucion del problema que tienes, debes actualizar el ensamble 

http://forums.autodesk.com/t5/Inventor-General/Inventor-not-updating-drawing-per-3d-modle-changes/td...

[Anonymous]

Hello,

I'm having the same problem that you described and some other questions. I normally use to a skeleton as a surface work piece. But, all of the sudden, when I insert this IPart in the assembly, it doesn't show anything! It appears in the browser, in BOM, but not in the window. Now, if I change to a normal work piece, with solid extrusions, it works fine. Why so? SOMETIMES, if i change the assembly to an IAssembly, it works out. But not all the times.

And I also wanted to ask, is there any way, using IASSEMBLY, to change the size of the frame? By clicking in the table?

Could some one help me out?

Thank you.

[lauris]

I have a very similar problem:

I've created a shell cube and a few lines as a geometry on which my frame is based. Assembly file is used to make a frame , using the edges of the cube:

When I want to change length or height of the cube, I change the sketch dimensions, from which the shell cube is extruded, and click ''global update'' button, so the whole feature changes with it. 

But the frame stays the pevious size.

Is there a solution to make it change with the cube?

[johnsonshiue]

Hi! The behavior is wrong. What Inventor release are you on? Could you post the files here or send them to me (johnson.shiue@autodesk.com)? I would like to understand why it does not update properly.

Many thanks!

[stevec781]

Still a problem in 2013.  You have to open the sub assembly that contains the frame and rebuild it.  A rebuild from the top level often does not cause a rebuild of frames in sub assemblies.

[lauris]

I sent the files to your email, 

I'm working on Inventor Professional 2015

[johnsonshiue]

Hi! I took a look at the files. I think I understand the issue better now. The skeletal part, Part1.ipt is also linked to top level assembly. Usually if the parameters are not driving geometry change across components, it should be fine. The trouble here is that the reference parameters in Part1.ipt interrupt the compute sequence. Reference parameters are supposed to be computed last because they are driven by geometry or other parameters. However, in this case, Part1.ipt has to be computed first to drive the frame members.

To prove my theory, simply delete the linked folder in the assembly parameters dialog. You will see any change in Part1 will propagate to frame members properly. Also, you can try linking model parameters, instead of reference parameters and the update will work fine also.

There is room for improvement in Inventor in this regard certainly, because the behavior is confusing and the user does not know what is happening. But, I am wondering why you need to link the reference parameters to assembly. Couldn’t you link the frame member instead? Or, you can create an assembly sketch and get driven dimension on project edges also?

Thanks!

[klemen_zivkovic]

This issue is very anoying - could somebody post an example of iAssembly that contains parameters, that drive Reference Skeleton?

So different values in table will change reference skeleton and update.

Here on my example I am using iLogic rule to transfer parameters of assembly to Part parameters. Reference skeleton is then linked to that part in frame.

But as others posted before - changing selected iAssembly in Table doesn't update frame accordingly.

This can be seen on screenshot bellow - so what is the right way of doing this scenario? The goal is to have parameters driven Frame and iAssembly.

Please post a little example to show concept of right way to do this.

[johnsonshiue]

Hi! Rule0 basically assigns the value of assembly parameters to corresponding parameters in the skeletal part. I am not an iLogic expert but I think there is a missing statement in the rule. There is a pending update in the assembly after the skeletal part parameters are changed. As a result, the assembly needs to be updated in order to reflect the change. Simply copy and paste the following to Rule0 and it should work as you anticipated.

doc = ThisDoc.Document
Parameter("Part2:1", "dolzina") = dolzina
Parameter("Part2:1", "visina") = visina
Parameter("Part2:1", "kot") = kot

MessageBox.Show(ThisDoc.FileName(False), "Opozorilo")
doc.Update()

However, there is an issue with the way the iAssembly was constructed preventing it from generating the correct member file. The issue is that the frame members are all driven by the skeletal part. These frame members are also shared by iAssembly members. If you try to generate iAssembly member files. The latter generated frame member will overwrite the former generated frame member. As a result, all iAssembly member files will be the same. If you are not using iAssembly member files, it may not be an issue.

Thanks!

[klemen_zivkovic]

Hi!

Thanks for answer but your answer/instructions didn't help.

Is your answer to be understand like there is no way for iAssembly to control reference skeleton? Please post solution to this if that possibility exist.

In mean time I went other direction - component copy in ordinary assembly.

I get 4 assemblies with lost connection of reference skeleton and part from wich skeleton was created.

This is very frustrating - so there is also no way to copy Frame Assembly????

Common Autodesk we are in 2014 - this is BASIC functionality (copying frame assembly with NOT lossing reference skeleton). It looks I should check SolidEdge ST 6. 😞

I couldn't attach sample since it is 6MB big.

[johnsonshiue]

Hi! Have you tried adding the Update request in the rule? If yes, does it not work for you? I was able to activate each iAssembly member and see the frames adjust properly. The latter portion of my prior reply is about the ability to generate member files.

The same frame member files are referenced by different iAssembly members. Essentially, you want Frame1 to be 12ft in iAssembly Member1, while the same frame member, Frame1 has to be 6ft in iAssembly Member2. However, Frame1's definition has to be unique. If you want a part to have a different length in a different context, there will be a conflict (should it be 6ft or 12ft).

I think what you need is to activate a member and generate the member file. Then, manually copy the iAssembly member file and all its referenced files (frame member, skeletal) to a different folder (not accessible by the iAssembly factory).

Please take a look at attached file. I made a copy of each member file and referenced skeletal part and frame members to a separate folder. Each iAssembly member behaves like an independent assembly. If there is any change within the iAssembly factory. You will need to go through the process of generating the member and copying files to a separate folder again.

Thanks!

[klemen_zivkovic]

Yes, I added so my rule is as follows (Vb.UpdateWhenDone = True line is there if this is what you meant by "Update request in the rule"😞

Parameter("skelet1:1", "dolzina")=ass_dolzina
Parameter("skelet1:1", "visina")=ass_visina
Parameter("skelet1:1", "sirina")=ass_sirina
'update all iLogic
Vb.UpdateWhenDone = True 

If I work in iAssebly and I double click on table - I can see skeleton and frame is changed accordingly.

BUT!

If I place iAssembly in another assembly and choose different rows in table while placing iAssembly in Assembly, both iassembly instances have SAME dimensions.

Further more - if I use "Generate Files" on table of iAssembly, generated files have same skeleton sizes - So how can I overcome this? Can rule be used in this at all???

So how can I controll this situation??

Can you post iAssembly that will change skeletons acording to iAssembly changed parameters?

[jalger]

Hi Klemen.Zivkovic,

I used " InventorVb.DocumentUpdate()" At the end of the my code.

I did one simple rule to update and sync the attributes.

-----------------------

Parameter.UpdateAfterChange = True
MultiValue.UpdateAfterChange = True

Parameter("Frame_Example:1", "Height") = Height
Parameter("Frame_Example:1", "Depth") = Depth
Parameter("Frame_Example:1", "Length") = Length
InventorVb.DocumentUpdate()
----------------------

I'm not sure if this is what your looking for but try out my sample Frame, it updates the frame members automatically.( it takes a few seconds for it to update)

For the Second issue, you could add the parameters to a Form and then the part would let you select the instance you want.

Any way here is the file and I hope it helps,

James

[klemen_zivkovic]

Hi jalger,

Thank you for sharing your solution, I tried it and it works while you are working in iAssembly.

When you try to "place component" - actually iAssembly in another ordinary assembly - than you get only assembly that is currently selected in iAssembly (check in table). So as the result you have 3 assemblies inside with SAME dimensions! Please confirm this!

Than as a consequence of this wrong behaviour later you can also select different active configuration in table of iAssembly (change chemark to different configuration in table), and you will see that all instances of iAssembly in test assembly change to latest table active configuration) - this is of course not what user would expect - do you agree? 

So please post picture of ordinary assembly where you have placed 3 iAssemblies inside - so asesembly with 3 Frame_Example_Iassembly and that results in 3 assemblies each with different frame dimensions.

regards

Zhivko

[klemen_zivkovic]

Anybody there?

Can somebody show how touse iAssembly parameters to generate different frames??

Is this all of the support we get from Autodesk?

[coreyparks]

This is a peer support group not meant for direct contact with Autodesk.  Many Autodesk employees regularly hang out here but they are by no means required to try and solve every problem found on the newgroup.  If you need to contact Autodesk directly working through your subscription page has worked well for me in the past.  There is at the least online support and depending on what software you own possibly phone support as well.

[johnsonshiue]

Hi! Did you take a look at my reply and the files attached to the message? Could you try it out and see if you encounter any problem? Like I said before, what you want is technically conflicting (a part needs to have different definitions but it has to be in one file). You cannot use the normal iAssembly insertion (generate member) workflow.

You have to manually make copies of the reference files. Actually, it is not much different than creating multiple assemblies.via Copy Design.

Thanks!

[klemen_zivkovic]

Hi johnsonshiu!

Hi! Did you take a look at my reply and the files attached to the message?

Of course I tried your sample. As I replied in previous post.

Could you try it out and see if you encounter any problem?

I tried - iAssembly works OK but when you put more asemblies in another assembly than it's not working.

Like I said before, what you want is technically conflicting (a part needs to have different definitions but it has to be in one file). You cannot use the normal iAssembly insertion (generate member) workflow.

You have to manually make copies of the reference files.

I tried that also - but in my case skeleton lost connection to part and than changing part in copied part it doesn't chang skeleton and therefore parts are left to be incorectly dimensioned. Skeleton simply looses connection to part in the copy process.

Actually, it is not much different than creating multiple assemblies.via Copy Design.

Thanks!

I wroted in previous post about it.

Yes I read it and followed it.

While you copy assembly - dont't your newly copied assemby skeleton keeps reference to the part?? CAN YOU PLEASE TRY THIS?

If it works for you what version are you on ?

Thank you

[klemen_zivkovic]

For anybody who still might be interested in this limitation of inventor 2015sp2 (loosing frame skeleton relation to part while user copies assembly), I workaround issue with creating normal part.

However this very much complicates my work - since now it's hard to me to get frame pipes specification in BOM.

For complex frame assembly  - you can imagine how hard it is to put whole frame in one drawing - ideally I would have each pipe in their own drawing and that would ease manufacturing or laser cutting of pipes later.

It's a shame but frame designer was so promissing... Can somebody from AUTODESK comment this frame designer limitation? OR maybe when this issue will be corrected?

Is there a list of bugs for autodesk where users can vote for fixes?

Or at least list of open bugs and/or won't fixes?

[Anonymous]

Press the REBUILD ALL button, and it will update. It's a temporary solution, but why doesnt it change after some time, is something quite usual in Inventor. NOT YOUR FAULT, Inventor details instead.