Linking Parameters between parts

[stephenson513]

hello there

So i have a box with a left side, right side, top, bottom and a door in an assembly.

Ive linked all the parameters to the 'right side component' so that when i change it, it updates all the other parts in the assembly.

What I want to accomplish is to beable to use my BASE SIZED BOX ( say 500 x 500 ) to create many different sized boxes.

The problem I have is when I save the assembly as a new one and save and replace all the components for the bigger box, all the components still reference the old part ( 500 x 500 right side component) instead of the bigger ( 600 x 600 right side component.

I hope you can understand 

What is the best way to do this kind of thing, Ive only just learnt how to link parameters, dont know ilogic, and just know the basics of assemblies and part modeling.

thanks

[karthur1]

You could mundge the name of the old linked file before you the new part, then when Inventor cant find it, you can resolve the link to the file you want.  Just remember to change the name back.  That is the way I used to do it.

Now, with iLogic..... I use this code (see attached).  When you run it, you can choose the new file.

Kirk

[stephenson513]

i will have to give that a try 

now with that code, should i create a new rule in the assembly and run it .... when ????

never done that sort of thing

[karthur1]

The way that I do it is to add a new EXTERNAL rule.  Then I can run it when necessary.  It does not reside in the part/iam and will always be available when you need it.

To add it, on the Mangae tab, click the iLogic Browser.  Then in the iLogic Browser, go to the External Rules tab and right click to add the new rule.

Next, go to the part you want to change the reference, then right click on the rule and then "Run Rule".

Kirk

[stephenson513]

that rule is amazing!!

This is how I do it, is it right?

1. I copy all the files

2. Rename them

3. Open the new assembly

4. Replace all the components with the new ones

5. Run the external rule and switch out the part that all the other parts are based off of with the new renamed one

6. Modify the size

works for me without changing the previous box 

now i just want a prompt that i can link the parameters of the base part to pop up so i can just change them that way instead of editing the part 

[yannicknielsen · Accepted solution]

Instead of replacing all the parts, you can just the Design Assistant.
Open your assembly and that, and all referenced parts will show up. Choose copy, and give them all a new name and place.

That way you're certain it all links to the new box, and you can then edit that box

[karthur1]

I take it you are coping and renaming these files in Windows Explorer... correct?  That workflow will work, but you "could" do the same thing using Design Assistant and it would be faster/easier.  Or, you could use Vault to do a copy design. 

If you used DA or Vault, you would be able to reference the correct file when you do the copy.

Don't know how you will get a prompt to tell you to change the size. If you dont like editing the part, you could reference a Excel sheet instead, but you would still have to edit it to make a change.  Using the Excel method, you can always reference the same excel file, you just change the starting cell.

Kirk

[mrattray]

We can make a prompt by using iLogic. You'll need to create new user parameters for each parameter that needs to be changed in your "base part". Then we'll create a form to edit the user parameters, then finally we'll need an iLogic rule to copy the user parameter's values into the base part.
OR
We can create the form in the base part. You'll have to open up the part in order to make changes, but we won't need any iLogic or extra parameters.

[stephenson513]

I checked out design assistant and it works pretty well. I didnt know about it.

when using DA does it mean i dont have to run the "replacebasepart" external rule that was mentioned above. will it automatically link all the new files in the assembly to the new "right side component "

[karthur1]

Right, If you use the DA workflow, there is no need to use the above mentioned iLogic rule.  If you swap out just the linked part and you need to change the reference, then you can use the iLogic rule.  That is sometimes quicker than using DA.... just depends.

The DA should relink all the files correctly.  Try it on a small test and see how it works.

Kirk

[yannicknielsen]

Design assistant will automatically make all files link to the new copies (if you remember to copy your skeleton, or base part, as well)

[stephenson513]

just a quick one here,

will this also work for .idw's

[IgorMir]

Hi guys,

Reading through all of these posts I want to ask - what, an old fashioned iParts and iAssemblies don't work any more? From the OP description - iParts would be the way to go, IMO.

Best Regards,

Igor.

[stephenson513]

Well you see, im not sure what those are.

I have not been taught those 

So I kinda want to know the best way. Maybe you could give me some insight on how that works

[IgorMir]

iParts and iAssemblies are well established features of Inventor. They have been discussed in depth on this forum too. May I suggest you search this forum first, than, maybe, have a look in Help file regarding that topic. After you do your home work we can iron out some wrinkles.

Best of luck,

Igor.

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@stephenson513 wrote:

Well you see, im not sure what those are.

I have not been taught those 

So I kinda want to know the best way. Maybe you could give me some insight on how that works

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