iAssembly / Table Replace

[Anonymous]

I am creating an iAssembly with iParts. Some of the iParts have the "Table Replace" colum option and some do not. Both iParts have tables with members and part numbers. See pic. Any advice?
wayne

[Anonymous]

I am going to reply to my own post.... I had to replace the component with itself because it was originaly inserted into the assembly as just a part then it was turned into an iPart.

[johnsonshiue]

Hi! The ones do not have "TableReplace" are iPart factory files. I guess the parts have been placed in the iAssembly or the original assembly before you convert them to iPart factory. iPart factory is the ipt file containing author table and all the member definitions. It is what you get when you convert a regular part to an iPart.
iPart members are the derive parts linked to the iPart factory. They typically are stored in a folder with the factory ipt name.
What you need to do is one of the followings.

a. Delete the iPart factory instances in the iAssembly. Place the factory ipt to the iAssembly again. At that moment, you will be prompted to place a member of the iPart factory.

b. Open th iPart factory in its own window. Select a member or a group of members in the browser->right-click-> Generate Files. Then replace the iPart factory in hte assembly with one of the members you just generate.

Thanks!

johnson.shiue@autodesk.com

[Anonymous]

Fantastic. This worked for me too.

[Anonymous]

Wayne's solution is elegant: rt click on part, select component, replace it with itself. It wiped out 2 of my constraints , but that took about 30 seconds to fix...aaaaaannnnnd now it works. Thanks Wayne!

[Anonymous]

Perfect, I also had this problem

[Zoltan78]

Hi!

I have the exact same problem. The only drawback of replacing a component with its iPart-self is losing about 20 constraint. Should I really know which parts will need to be iPart in designing stage? They should have really solved this years ago - Inventor 2015 acts the same.

[Anders.nelsonZH4PE]

Still haven't fixed it.  Come on AutoDesk!!

[johnsonshiue]

Hi! This is a very old thread. Your comments are not actionable. Please start a new thread or provide an example showing the exact problem you are having with iAssembly.

Is it about trying to use Table Replace of an iPart factory within an iAssembly? If yes, Table Replace does not work with iPart factory. It is because iPart factory contains all the member definitions but it cannot exhibit itself as multiple members at one time. What you see in an iPart factory is simply the active member on the table.

Many thanks!

[Anonymous]

Update on this issue for May 2019 (running Inventor 2018) . . . Wayne's fix of manually replacing the part file with itself is still the needed workaround.  

The iAssembly will not recognize if an existing part file in the assembly has been updated to become an iPart file.  The "table replace" option won't become available until the part file has been manually replaced.  

Other fun bugs with replacing a part with itself:

- broken mates for no reason - there were no changes to the part or existing features.  I only created an iPart variation that suppressed two holes that did not interact with the mating feature.  

- Loss of custom names to planes - I had added a note on the XZ plane title in my part for easier identification for mating.  The custom note was no longer visible in the assembly feature tree after I had replaced the part with itself.  

[johnsonshiue]

Hi! The main reason users are seeing this behavior is because the process of building up iAssembly and iPart are not clearly stated. iAssembly and iPart are meant to be library components. You need to start with iPart. Make sure all iPart members are generated. Then you create iAssembly based on the iParts or other parts.

When you try to convert an existing assembly to an iAssembly, you will run into the issues you are talking about (broken constraints or loss of references). You will need to replace the existing parts with the iPart members. And, fix up the failed constraints. Another technique to use is to create iMate instead. However, there is yet another "after-thought" process. If you don't have iMates in the first place, you need to create iMates and then recreate the constraints. I have to agree the process is confusing and it is not user friendly.

Many thanks!

[Anonymous]

@johnsonshiue :

in your last post you mentioned that an iAssembly should include iMates. Now I am creating an iAssembly that consists of a motor and the various assemblies.
Now I just made all the constrains but no iMates applied. If the iAssembly is tested separately it works but if this iAssembly is placed in an assembly and constrained to the frame, the iAssembly still works but when I change component of the iAssembly error messages appear from some constrains. If I recover it top-down, I even get an error message in the iAssembly. Does this have to do with iMates?

Regards, Joop

[johnsonshiue]

Hi Joop,

I will need to see an example. I guess either the iMate is not at the individual component level, or there is a matching error. Please share the files here. I would like to understand the behavior better.

Many thanks!

[sanelP52]

it is still the same problem in 2022 version ...
btw. thanks Johnson for all of your answers on various topics.
I learned a lot from you.

[Anonymous]

I also have the same problem when replacing a part with an ipart, it creates errors on all the related constraints !  

[johnsonshiue]

Hi! iPart/iAssembly are meant to create reusable library components. To keep the constraints intact in iParts, you may want to use iMate (name/type match as opposed to geometry match).

Inventor 2022 Model States should help this case. It is because the geometry variation is all wrapped within the same file as opposed to separate member files in iPart/iAssembly.

Many thanks!

[raja.dahya]

this issue is non-existent in SW. as soon as you make a part a configuration, that is filtered into any assembly it is part of. heavily increasing model time Autodesk??

[Zoltan78]

I bet SW has other issues. I've worked with Inventor for 15 years and there were no issue that couldn't be handled and would set my work back much. Thanks to its support, its community and their very clear online help.

[raja.dahya]

I'm not saying SW is perfect. it has plenty of glitches. but it has so many convenient features they have added intuitively over the years that make it vey easy to deal with. No need for "work arounds". I had high hopes moving over to inventor but its very 'old school' in my opinion. And for every question I look for in the forums, the only answer is usually a "work around".

[Anonymous]

I agree with Raja.  I've been using Inventor every day for more than 3 years now.  There are still things that I figured out in a day or less in Solidworks that I can't do (or will avoid doing after seeing how cumbersome the workaround is) in Inventor.  Everything I was trying to do with iparts and table replace would have been a complete non-issue using SW configurations.