How to link the ipart members in to new part file

[ramkrish]

Hi all,

i have facing issue to link the ipart members in to the new part.

for example,

i have one machining part that machining part showing  make from number. so, i created make from first. it has 10 instance.using iPART i created 10 members.after that i need to be do the machining.machining drawing also having 10 members. how i call the each make from members in to the machining model.please give your valuale reply.

for detail please find the attached image file.

thank you,

regards,

ram

[MariaManuela]

Hi...
Image please 🙂

[ramkrish]

i am realy apolozies

please find the attached document

[ramkrish]

i browsed the location but attachment is not added.

i don't know why it is happening.

[MariaManuela]

[MariaManuela]

Try Insert the image, not attach

[IgorMir]

Hi Ramkrish,

You have to consider two options:

1. If you derive the Factory file (the one which has iPart table) into a new file then every time you change an active member in the Factory file it will be reflected in the file in which it is derived to. (I hope it makes sense to you )

2. If you derive a child, produced by the factory file - then only changes to that child will be propagated to a file which contains that child. Changing the active member in the Factory file will not have any effect to the derived component.

Ideally, when the Factory file is derived to a new file we should be able to select an iPart member from the table, as we do when creating iAssemblies, for example. It has been discussed before, BTW. But I don't think anything has been done to achieve that. Not to my knowledge anyway.

Regards,

Igor.

[dcmorgan]

I to have ran across this issue in Inventor. I have created an Ipart table with 10 or more instances in it, and then tried to create the finish grind file by deriving the Ipart itself into a new ipt. But just like IgorMir mentioned, this will not work due to the fact that the file changes based on whatever is active at the time.

Another work around for this besides the ones mentioned in this forum is to cross reference raw and finish values in the table using EXCEL:

Create the raw and finish file in the same table. To avoid having to re-enter information for finish part, you can open the table in excel and reference all the raw values that apply to the finish cell dimensions. Since the finish part only has a ground surface, that would be the only values that would differ between the two in the table. This way when you change the raw dimensions in the table, the finish dimensions will update as well. Once you reference a dimension to another using excel, that box should be grayed/red out not allowing you to change the value unless you change raw value in Inventor. So far this works great!!!  This in essence is accomplishing the same thing as a derived ipt part file.

I hope my explanation is clear. Attached is a screen shot of my table. The ones in red are finished part file. The grey cells is the raw part file