Inventor Part Configurations

[Cadmanto]

Ok, in Pro-E they are called instances, in Solidworks they are called configurations.

What are they called in Inventor and how and where are they created.

In Solidworks you create what is called a design table that create's similar but

different parts maybe only varying in lenght or color to name a few differences.

Just trying to figure out how to do this in Inventor.

Thanks for your help.

[ampster401]

look up something called "iParts" and possibly "iAssemblies"

[mflayler2]

Or you can use iLogic, it just depends on how much configuration you want to accomplish.

If it is only 20 parts and will only ever be 20 part variations, iParts are not a bad choice.

If you are continately updating the table for new configurations or new variations of known parametric value, then iLogic should be a better choice.  For instance if you have a value in your table that is always in flux (value could be somewhere between 2 and 20 and the actual value is anything the customer wants between), you wouldn't want to make to large of a table to accomodate this you would want a configurator instead which iLogic will do and also allow you to create a form for the logic.

[JimSteinmeyer]

Scott,

IParts and IAssemblies is what you are looking for and they kind of work llikke SWx. The thing I am still having problems with is that I have edited a couple of IAssemblies after creating a drawing and am having a hard time  getting them to update in the drawing without reinserting the view in the drawing. I keep getting a message to open the Factory (what I think they call the top level assembly) and then regenerate the factory members ( the different IAssemblies) I keep trying to do this to no avaol and have not been able to find any suggestions on how to solve it.

Good luck

Jim

[Cadmanto]

Thanks Jim and Mark.

I will be looking in to the iparts and iassembly.  Sounds definately what I am looking for.

[mflayler2]

Also, make sure you read up on how iParts and iAssemblies create files.  Unlike the other software, in Inventor each row of the table will create a Derived part variation of that row.  So if you have 20 rows, you will end up with about 20 seperate part files so they are all uniquely trackable and and revision-able.  This makes the PDM tracking availble for individual files rather than a single part which can cause problems in the other software for tracking.

[prachu]

Sounds like the same thing I am just kinda figuring out. When you insert a part with multiple configurations into a drawing, Inventor makes a sub folder with what is essentially a copy of the part in that specific configuration. Every time you add a different configuration of that specific part to a drawing, it will add it to the sub folder.  When you make a change to the top level part, that change doesn't automatically propegate down through all the "copies" that the drawing references. In order to update the drawing views, you need to go into the sub folder, open the specific configuration for that drawing view and then do a "local update" (located under the "manage" tab).

It is annoying and I'm not sure why Inventor can't update all the iparts when you make changes to the top level part. It's one area of Inventor that I much prefer Soildworks methods for.

[mflayler2]

You could use Generate Files to create all the parts for you right away instead of waiting for when they are actually placed from the configuration.  Granted it is more work on the modeling side, but in documentation it is the preferred method.  For some reason the other software vendors think it is okay to have 20 parts actually only be one modeling file.  For me that is a documentation nightmare!

[cadman777]

iparts and iassemblies don't seem like a good work-flow for what i'm trying to accomplish.

if someone has created a good workflow for what i'm trying to accomplish, please advise:

objective:

make parts so that they can be used in 4 kinds of drawings:

1. material prep = rough part cut out of stock

2. pre-machining as a part

3. weldments (i.e., assembly file)

4. machining of the part in the weldment (i.e., assembly file)

the problem i have with assembly features is they disappear when the assembly changes, which means i have to begin anew to creat them, and fix the drawing views in which they appear. this is a big headache and lot of unnecessary work.

so if the pre-machining and machining features can be embedded in the part, and referenced along the way in the assembly file and various drawings, that's good.

however, i haven't figured out how to do it that way.

that's how it works in SW.

why do i use IV instead of SW?

b/c the work-flow is much better in IV for the kind of work that i do, except configurations.

plus, SW use of metadata "sucks" (= IV parameters and fomulas), and the SW developement people don't want to hear about it. if the crowd ain't saying it, then it's irrelevant to any "wish list" items. whatever ...

so, i'm not going to waste time WAITING for SW to get up to speed w/my needs.

still, i need IV to do some stuff that SW does: configurations.

any good advice would go a long way ... chris

[SBix26]

(A new thread would have been helpful so others searching would find this topic more easily).

I think that I would try this with multi-body parts, as follows:

In a part file, create the material prep part.  Pattern this a convenient distance & direction, selecting "Pattern a solid" and "Create new bodies".  Then on the patterned part, do the pre-machining operations.  Derive these (Make Part or Make Components, or manually) into two separate parts which can be detailed individually.

I'm not sure why your machining features in the weldment don't survive part changes, but it may have to do with the iParts.  If that's the case, then the multi-body approach may help with that.

[cadman777]

Thanks for the idea, Sam.

I never would've thought of using "pattern solid". I believe the work-flow involved would complicate things too much down-line.

The work-flow I came up with in the past is a bit more complicated at the outset, but has few problems down-line, unless I use assembly features. The reason is b/c I always use primarily "wireframe", and a little bit of "muscular" modeling.

What I've done in the past is create a wireframe model with all the as-machined workplanes.

Then I make the "stock" part thicker and larger based on machining allowances.

Than derive the "stock" part and do preliminary machining on it, such as tap holes, openings, slots, grooves, etc.

Then make an assembly (which is a weldment without using the "weldment" module) with all the preliminary-machined parts.

Then do final machining on that assembly.

It's got its caveats, but it seems to have the least amount of problems.

Also, there are variations to this, but that's pretty much the way I figured it out.

About "Threads":

I was 'scolded' in the past for starting new threads on subjects that already were being discussed.

Hence, my use of an old thread that seemed to fit my situation.

I guess, from now on, I'll start new threads and reference old threads if need-be.

Cheers ... Chris

[SBix26]

Give the multi-body solids a try.  I did a simple weldment of two such parts, added a machining feature to it which depended on projected edges, then modified the part.  The weldment adjusted without a problem.  What kinds of complications do you foresee down-line?

[cadman777]

Sam,

MBP is a great idea.

I've used it in the past for small weldments, like davit-hung tank doors/manways (that weld to a tank GA) and control panels/consoles (that are part of a bigger sheet-metal cabin), etc. Works great.

Never thought of using it in this process.

I'm currently "experimenting" with ideas and work-flows in order to arrive at the most simple and "worry-free" method.

Since I use wireframe base files to drive all my parts, this sounds like another workable option.

Can you post your MB part for me to take a look at?
This is the kind of discussion this forum is really good for.

Thanks ... Chris

[SBix26]

What version are you using (put it in your signature, then nobody has to ask)?

[cadman777]

Good idea.

Let's see if it worked.

[SBix26]

The signature worked.  But I don't have 2010 any more, my files are 2012.  Sorry.  They're all zipped up ready to go, but they won't help you if you can't open them.

[cadman777]

do you have any from IV2010?

[SBix26]

Nope, sorry.  I didn't really understand the power of mult-body stuff until the last year or so.

[cadman777]

no probs ...

[Patrickwesc]

yes, its much easier to update 20 individual files then it is to make one change and push it across all configurations.  You must be very busy wasting all that time.....