Assembly driven Parameters to resize child components

[Anonymous]

Is it possible for you to create a set of User parameters in a parent, such as Length, Width and Height, and have the children absorb these parameters as their constraints? I keep getting "cyclical dependency" if I try to link a child to the parent.

This was possible and simple in Solid Edge.

[karthur1]

I take it in the part, you are using the "Link" comnmand in the parameters dialog and browsing to the assembly file.  If the part is used in the iam, then yes, you will see a cyclic dependency error.

One way around that is to create a .xls sheet that has the parameters that you want to share between the two and use that instead of the iam.  Its an extra file that you have to keep up with, but it will work.

[CadUser46]

I have wanted the same thing.  From memory if you expose the parameters in the child they are visible in the parameters of the parent?  It would be great when doing skeletal modelling if you could edit the parameters from the parent and drive them back down into all the referenced children.

[jtylerbc]

Another way is to use a Layout part for this purpose instead of the Excel file.  This part can also be used to contain geometry to help control the model (sketches, reference planes, etc).

We build a lot of welded assemblies of steel plates, and a combination of layout parts and multibody parts is my usual way of modeling them.

[CadUser46]

jtylerbc, i currently do the same thing.  I make the first part in a fabrication a dud part basically just filled with all the parameters i want to drive.  Even re-name it to 'Parameters' so its obvious to other users that pick it up later.

It would just be a little bit slicker if you could make the edits in the assmebly parameters rather than going down into the edit of the part.  Actually i think it should be possible to edit the pararmeters from any part/assembly they are linked to/visible in.  Naturally if a user cross linked it to other parts/assemblies this could cause problems with tracing all the links.

[jtylerbc]

I agree that it would be easier, to the extent that I've tried exactly what the original poster attempted with linking to the assembly in cases where I didn't need the "skeleton" to contain any geometry.

I fear, though, that just like you said, the link tracing could easily become a nightmare.  I suspect it's one of those things that would seem like a wonderful idea until you had the first one go horribly, horribly wrong.  No system I've ever used had the ability, so maybe I'm overstating the problem, but it just seems to me that it could go badly.

For now, I don't mind the "Layout" part too much - I just make sure to keep it at the top of the browser where it's easy to find, and often have it open in another tab when I'm working on the assembly.

[swordmaster]

Look into Ilogic it is built into Inventor 2010 and upwards (an add in for Inventor 2009)

You can have your parameters in the top level assembly and use ilogic rules to send the values from the upper level to update the part parameters.

There are two tutorials that come with the Install that explain the process in more detail

[Anonymous]

As I mentioned in my original post, the method of centralizing design driven parameters within the parent assembly and linking each child component to alter it's values was simple and easy within Solid Edge. That being said, if you failed to copy existing parent/child heirarchy's by using Solid Edge's Revision Manager, then yes, the links would definately get "lost".

But when a proper design copy was performed, the whole parent/child integrty was maintained and proved a very valuable tool to centralize design parameters for such types of products in which that was permissable.

That being said, I've opted (in this case) to utililze the Excel link option, as the output the spreadsheet is something that has been around for years and is full of many, many formulas that I would have to recreate within the alternative option of a "dummy" part. But for new designs with limited formulas and derivitives, I would opt for the "dummy" part.

Thanks for the input everyone.

[jtylerbc]

swordmaster,

Slight correction - not built in to 2010.  Still an add in (only included with suscription, I believe).  Built in to 2011.

Sadly, I know this because I'm on 2010 without suscription, so no iLogic for me.

bmlkidd,

Solid Edge isn't one of the systems I've used, but I can see how that feature would be useful as long as you were careful enough not to hurt yourself with it.  Other than editing iPart tables, I don't have much experience with using Inventor and Excel together.  Also I usually have some use for sketches and reference geometry in the dummy part, so it lends itself better to my models than Excel typically would.  Also, since my company is relatively new to Inventor, I fear that someone would see the Excel sheet in the Inventor folders and delete it thinking it was there by mistake.  Hopefully they'd be more cautious about nuking an .ipt file.  Hopefully.

[Anonymous]

Yes, I've considered that a fear as well (deleting the Excel file). However, I have observed two things:

1. We use Vault, so non-engineering personnel will never see any Inventor files

2. There is an option to 'embed' the Excel file within the assembly, so I will investigate that as an option.

I, too, am new to Inventor, coming from Solid Edge for 9 years, from UG for 3 years, CATIA for 2 years, blah blah blah all the way back to an old system called CALMA, which was back on the mainframe days and when the computing term 'workstation', actually meant furniture and hardware manufactured together. I've seen a ton of progress over the years, and back 25 years ago, I would never have envisioned the capabilities that we have in front of us today.

One other kind of off-topic note:

Solid Edge had a tool (prior to Synchronous anyway) called Adjustable parts. This was an awesome utility that I used every day. Here's how it worked.

1. You create a part that you know you will always need, but with a varying parameter (variable in SE).

2. You assign which parameter(s) where to be adjustable in upper level assemblies.

3. You place the component as adjustable and a dialog lets you enter the desired value.

Doesn't sound like much, but lets say you have a part you purchase, such as 4" sch. 40 pipe under, lets say , P/N 200-010. Now everytime you need to reference that purchase part number, you typically create a new file that depicts the correct length, and maybe append the actual length to the end of the file name (ie: 200-010_18_in_lg).

If you have 600 version of length of this part, you have 600 part files. Imagine you need to change a property in this part number. Phew.

The beauty of the Adjustable part was that it DID NOT create a new part for each instance, it simply altered the instance within the upper level assembly. Thus, only ONE part file actually existed.

May not sound like much, but was a really wonderful feature. As far as I can see, the closest thing would be iParts, but it creates not only extra files, extra folders. If anyone is still reading this, do you know a different method?

[jtylerbc]

It's the engineering staff I'm afraid of - this is still mostly an AutoCAD company, so other than the occasional XRef, they're not used to thinking in terms of links between files.  I've personally used Inventor for several years, having come from another company where it was the standard.  That's not the case with most of the other personnel here.

It looks to me that the function of your "Adjustable" parts in Solid Edge is somewhat split between iParts and Adaptive parts in Inventor.  Neither does exactly what you're describing, since iParts create the extra files and Adaptive parts can adjust, but only to one situation at a time.  In other words, they adjust to changes in the assembly automatically, but you can't have an instance 1" long and an instance 12" long - that would require two adaptive parts.  There is no direct equivalent to the feature you're describing, as far as I am aware.  I've seen lots of cases where I could have used something like what you're describing.

If pipe or structural steel is the actual case, and not just an example you picked, you might want to look into the Frame Generator.  It still creates a load of part files, but it manages them for you, for the most part.  Along with a bit of customization to the Content Center to get numbering and description formats to match your conventions, I think that would be the closest thing.  We do a lot of fabrication using steel tube, and I've had pretty good results out of Frame Generator for that type of work.

[CadUser46]

Unfortunately Part Represenations is something Inventor users have been asking for for ages.  Other than the way you have suggested there is only the one other method i can think of that is vaguely similar.

We have lets say a template for box section.  The actual BOM is driven from the custom Iprops which we populate via PDM.  This allows us to create seperate models for the same part number but with different lengths.

Be wary embedding excel files unless you plan to stay within the Autodesk family forever.  They could create a migration nightmare if you choose to integerate with certain PDM systems unless you are using unique file names.