Multiple options for a general design

[Anonymous]

Hello Autodesk community!

I have tried searching the web and could not find a direct answer, can someone please help!

At the company I work for we have designed a product that has multiple options and we are looking for a way to copy the main model and drawing for that model and adjust the model per the different variations, and at the same time update the drawing.

Right now we have to take the main model, copy it, save as a new part number then change features to the customers specification, then redo the entire drawing just to specify a minor height change or diameter size. Its pertinent to have separate part numbers due to customers ordering the different variations in the future.

We want to be able to take the main model, give it a suffix part number, modify it and not have to redo the drawing.

FOR EXAMPLE:

MAIN ASSEMBLY PART NUMBER - ABCD

COMPONENTS OF ABCD-            -##

ABCD.IAM

ABCD-01.IPT

ABCD-02.IPT

ABCD-03.IPT

ABCD-04.IPT

ABCD.DWG

A CUSTOMER REQUESTS THAT THE -02 BE A CERTAIN HEIGHT

ABCD-AA.IAM

ABCD-01-AA.IPT

ABCD-02-AA.IPT

ABCD-03-AA.IPT

ABCD-04-AA.IPT

ABCD-AA.DWG 

A CUSTOMER REQUESTS THAT THE -01 HAS A LARGER DIAMETER HOLE SIZE

ABCD-AA.IAM

ABCD-01-AB.IPT

ABCD-02-AB.IPT

ABCD-03-AB.IPT

ABCD-04-AB.IPT

ABCD-AB.DWG

HELP PLEASE AND THANK YOU!

[Curtis_W]

Hi @Anonymous, 

Welcome to the forum. I know kelly.young started this "Ask Anything..." thread to invite questions, but in the future you'd be better off to start a new topic of your own. But that's a minor point.

As for your question:

If you have Vault there is a Copy Design tool that allows you to copy the drawings, assembly, components, etc. all in "one fell swoop", if you do not have Vault, you can use the iLogic Design Copy tool to do pretty much the same thing. Note that your files do not need to include any ilogic code to use this tool.

See link:

https://cadsetterout.com/inventor-tutorials/copy-an-autodesk-inventor-design/#ilogic-design-copy-too...

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[Mark.Lancaster]

@Anonymous

Welcome to the Autodesk User's Community..

Three methods come to mind..

1. Create an Ilogic interface.  Do you know how to program using iLogic in Inventor?

2. Use the iCopy tool (Not sure what your model consist of, but it could be option). https://synergiscadblog.com/2015/11/23/inventor-icopy/

3. Use the iLogic design copy and copy your model template/drawing for each job. https://synergiscadblog.com/2014/09/23/copy-files-easily-with-ilogic-design-copy-even-without-ilogic...

[jtylerbc]

Design Assistant can handle this as well. 

If you have any that are already in process, but haven't had the drawing created yet, you could copy an existing drawing and use the "Replace Model Reference" tool to change which model the copied drawing is looking at.  This would be kind of a crude, brute-force method that I wouldn't recommend for future design variations, but if you have any that are partially complete it may be the easiest way of finishing them up without having to completely redo the drawing.

[kelly.young]

Hello @Anonymous I see that you are visiting as a new member to the Inventor Forum.
Welcome to the Autodesk Community!

How many people are in your company and how do you handle revision management and sharing files?

Depending on your needs you might want to research implementing the Vault.

Here are a few posts with good links on how to go about copying a design:

how to copy a subassembly

Inventor Create New Assembly Member Sizes Without Recreating Parts

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

[johnsonshiue]

Hi! I think you could probably do Selective Copy Design workflow. You don't need to replicate the entire assembly and parts and put them in a different folders. What you need is simply open the assembly file and save as different iam files. In each assembly, swap out the part which needs to be different (Replace Component). You can also rename the occurrence names in the assembly.

For drawing, you can create drawing views based on one assembly and annotate it. Then save the drawing file as different drawing files. Then use Replace Model Reference command to redirect the drawing views to different assemblies.

Many thanks!

[IgorMir]

Reading all the replies I couldn't help but wonder - what, iAssemblies and iParts are out of fashion already?

From what the OP has described - it seems to me iAssemblies and i Parts would be the way to go...

Cheers,

Igor.

[johnsonshiue]

Hi Igor,

Indeed, this is debatable whether iPart/iAssembly is a suitable workflow here. It does seem like a logical choice for simple parts and assemblies. However, if you are designing multi-level assemblies, you will see iPart/iAssembly may not be a good workflow choice.

The main roadblock is within iAssembly. The iAssembly BOM table only allows first-level components to be shown. There is no "all-level" or "part only" view. This makes documentation difficult. You can get over it by placing the iAssembly member to another assembly for BOM table. But, it adds yet another file to manage.

For iPart, unless each member has clear definition and it is totally driven by the table, iPart may not be helpful. You will end up managing a large table with many members and rows to accommodate all the needed variations. In the end, each member is still another ipt file.

In my mind, iPart/iAssembly is best for out-of-context configuration. It means these components are clearly defined and they don't need to change based on where they are at. Things like nuts and bolts, actuators, and motors. On the other hand, they are not good for in-context configuration, meaning the components will need to change shape in different assemblies and these changes apply to one specific assembly context, not to others.

Many thanks!

[IgorMir]

Hi Johnson,

Yes, if assembly is very complicated - using iAssemblies might present some logistical issues. But then again - Copy Design creates a whole new set of files as well. Which are just as cumbersome to manage as it might be with iAssemblies.  Hence - the decision which technique to use to control the design would be based on a company's specific requirements/preferences.  Let's see what OP thinks of that.

Cheers,

Igor.

---

@johnsonshiue wrote:

Hi Igor,

Indeed, this is debatable whether iPart/iAssembly is a suitable workflow here. It does seem like a logical choice for simple parts and assemblies. However, if you are designing multi-level assemblies, you will see iPart/iAssembly may not be a good workflow choice.

The main roadblock is within iAssembly. The iAssembly BOM table only allows first-level components to be shown. There is no "all-level" or "part only" view. This makes documentation difficult. You can get over it by placing the iAssembly member to another assembly for BOM table. But, it adds yet another file to manage.

For iPart, unless each member has clear definition and it is totally driven by the table, iPart may not be helpful. You will end up managing a large table with many members and rows to accommodate all the needed variations. In the end, each member is still another ipt file.

In my mind, iPart/iAssembly is best for out-of-context configuration. It means these components are clearly defined and they don't need to change based on where they are at. Things like nuts and bolts, actuators, and motors. On the other hand, they are not good for in-context configuration, meaning the components will need to change shape in different assemblies and these changes apply to one specific assembly context, not to others.

Many thanks!