3D sketch iPart for rack design

[Anonymous]

I'm trying to build a rack based off a 3D sketch and make it into an iPart. This is proving very difficult without doing a bunch of work arounds that are more time consuming and restrictive. 

I have 11 racks that will share the same common design but have varying outer dimensions. What would be the easiest way to do this? I want to be able to have a base sketch, use the frame generator, and just create multiple instances of this design but with the varying dims. 

[mcgyvr]

Can you post this 3d sketch file?

[Cadmanto]

Can you also post some pics of what your trying to make?

Windows 10 x64 -16GB Ram
Intel i7-6700 @ 3.41ghz
nVidia GTS 250 - 1 GB
Inventor Pro 2018

[Anonymous]

So the idea was to use this 3D sketch, which has an iPart table. Create an assembly, thus allowing me to pull the multiple instances into drawings with a change in the dimensions with the click of a button. However when you try to add the 3D sketch/iPart into an assembly, it does not show up. Now I know this is an issue that's been out there awhile and there are several work arounds but they didn't really seem to work without adding a ton of work anyway, thus making it more efficient to just model the 11 instances individually. I'm trying to not to have to do that, so is there a better solution? 

[Anonymous]

Base frame will have a ball roller top and adjustable feet and floor anchors added as well

[johnsonshiue]

Hi! It should work if everything is confined within the iPart. If you are trying to use iPart as a skeletal for a frame assembly, or, you want the frames to be iPart members driven by a skeletal part, you will run into trouble,

iPart/iAssembly are meant to create library contents. Basically, the definition of each component is well defined and explicitly laid down on the author table. Any attempt to drive iPart/iAssembly outside of the table will not work properly.

Many thanks!

[Anonymous]

Ok got it, that's what inventor can't do. Is there a solution achieve this table driven design?

[johnsonshiue]

Hi! I think you will need multiple skeletal parts and multiple frame subassemblies. iPart/iAssembly is not a good solution to what you are trying to do. Here is what I would do.

1) Create a frame assembly for one configuration and save.

2) Use iLogic Design Copy (close all files -> Tools) to create another dataset.

3) Open the newly copied assembly.

4) Alter the parameters manually or use iLogic rules to drive parameter changes.

5) Repeat step 2 to 4 for other configurations.

Many thanks!

[kelly.young]

Hello @Anonymous to add to what others have stated, here is a quick overview on how to get the 3D Sketch into a parametric state where you can drive it with an iLogic Form.

If you are using Vault or the iLogic Copy Design tool you can easily create different instances of the model and rename to individual parts. 

Please select the Accept as Solution button if a post solves your issue or answers your question.

[Anonymous]

Turns out this doesn't quite do what I was wanting. When you do a "Save as" and rename the initial table assembly as "Table 1, Table 2, etc" they will still refer back to the same Frame members. So when you update a Assembly size in one, the change is also registered in the other assembly. I tried going through and saving unique wire frame sketches and changing the iLogic rules to reference those, but unless you delete all the frame members and give each table assembly their own unique set of frame members, any size changes will update across all models referring to the same frame members. Pretty much making the whole process of iLogic useless since I'll have to go into each table assembly and create unique frame members for each assembly to have unique instances of size.

[kelly.young · Accepted solution]

@Anonymous you are correct in that SaveAs will not replace the Frame Generator components, you need to use the Vault Copy Design or iLogic Design Copy to achieve a duplicate to work with.

If there is something else you are trying to achieve let us know and see if we can point you in the right direction. 

Please select the Accept as Solution button if a post solves your issue or answers your question.

[Anonymous]

This should do the trick, thanks for the help