Configuring parts list

[Anonymous]

I'm having a difficult time finding exactly how I set up the parts list table. I'm thinking that I must have the wrong terminology when searching.

A background on exactly what I am trying to accomplish. I am a cabinet maker and have made the final decision to use Inventor for my design program. I'm taking the self learning method and I get most of it, I feel like I'm on the edge of a breakthrough, but I seem to be stuck on the parts list and getting the information I need.

For a basic example, a shaker door. It has 5 parts; 2 stiles, 2 rails and a flat panel. I need to have the dimensions pop up in the parts list for all my pieces. Just basic length, width, depth, dado, etc. I guess that I felt it would be a piece of cake to configure Inventor, but for the life of me, I cannot find the information I need to go from a part file to shop drawings with dimensions and details.

I also need to make sure that I can get the driven dimensions to show up, since the rails (to the best of my knowledge) have to have driven dimensions. I assume that this is possible. 

What I am trying to accomplish is something like what cabinet vision produces for documents. I chose inventor for the flexibility of design since I do some unusual things with cabinetry and cabinet vision just can't handle it.

I really appreciate the help, I apologize for what is probably a simple question. I've been digging for answers for about a week to no avail.

[jtylerbc]

Don't feel bad - I know how to do it, use it almost every day, and still had trouble finding directions in the help files to show you where to find it.  Instead, take a look at the attached document by Mark Flayler - I believe it will cover most of what you need.

The key things are to:

1)  Name your parameters

2)  Mark the parameters as "export" to turn them into iProperties

3)  Format the exported values with the desired units, decimal places, etc.

4)  Create expressions to embed them in your part description

The document will detail exactly how to go about doing those things.  Once you figure out how to do it, I'd recommend creating some custom part template files with the work already done, so you don't have to keep redoing it on different models.

Hope this helps.  Post back if you have any trouble.

[Curtis_Waguespack]

Hi k-dawg,

What version of Inventor are using?

How familiar are you with Multi-body parts, the Make Components tool, and iLogic?

I have an example I can share, but I thought I'd get some background information first.

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

[Anonymous]

2012...and I have your book! Well...I could only find the 2011 edition of Mastering Inventor.

I would be at the rookie level. I have worked with a few other Autodesk products, but not to a mastering level. 

I am familiar with the terms, but I don't know all the nitty gritty details on how everything connects together in the program. I have read up some on the guy who was using iLogic with the cabinet and was trying to follow as much as I could, but I got lost after awhile. 

Do you have a suggestion on my workflow?I guess I fear most that I will start making part files to my liking and later find that I wasted all my time. 

I read through this thread to get some ideas for which tools to use in Inventor and like I said, I'm still trying to connect the dots. I was so stuck on this one thing for some reason. After reading the white pages posted by tylerbc, it's making much more sense now.

http://forums.autodesk.com/t5/Autodesk-Inventor/Inventor-for-Woodworkers-Joinery-Millwork-and-Cabine...

What I am going for is something that prints out for the shop, but in a much more customized way. I am trying to accomplish something like cabinet vision, but better. This is an example assembly sheet that prints out from CV.

http://esupport.cabinetvision.com/help/solidhelp/room_level/side_bar/Assembly_Sheet/RLSBAS_Layout.ht...

I wanted to make sure before I went too far that I was able to get those specific dimensions on the shop drawings, which I assumed would be more than possible. The other parts would be quick, ease of design (which I feel I have a decent handle on, just more practice needed) and visualization. Kind of a combination of 2020 and CV with decent renderings.

I assume that there are still yet much easier ways to accomplish what I am looking for, and I know that I have my work cut out for me since I need to make my own library of parts, but I have this gut level feeling that this was the correct way to go for what I need for my shop.

Believe me, I am grateful for the feedback. It was killing me just finding the parts list configurations. 

Kent

[Anonymous]

jtyler, thank you. That was exactly what I needed. I got what I needed where I needed it. A little fuzzy on the iProperties expressions and how that helps me.

• Got the parameters down
• I understand the difference between model, reference and user parameters
• I understand that I need to work on and configure my parts list style
• I think I understand the iPart...at least enough to do what I need it to do
• I understand that I need to work on my templates so I don't keep repeating things
• Have not looked into the BOM fully or expressions

Just out of a passing curiosity, when I get to assembling all of my cabinetry in an .iam, I am figuring that I have to model my mouldings there. Crown, light rail, etc. Not sure how that all will tie into my parts list.

[jtylerbc]

Where the expressions help you is in embedding dimension values into the text of other properties.  For example, let's say you have a panel whose Description field needs to be:

PANEL - LENGTH X WIDTH X THICKNESS

You could set up the parameters LENGTH, WIDTH, and THICKNESS, exported and formatted with the appropriate units and precision.  Then in your Description field, you would enter:

=PANEL - <LENGTH> X <WIDTH> X <THICKNESS>

This would result in a description that contains the values for those dimensions automatically, and updates when they change.  I use a similar setup for rectangular steel plates.  I then saved a copy of one, with arbitrary values for the dimensions, in my Templates folder.  That way, any time I need a rectangular plate, that work is done for me, and I only have to size it by changing the parameter values.

Moulding isn't something I deal with, so a fellow wood/cabinetry designer might have some better ideas.  One that comes to mind for me is making your moulding a custom iPart, with the length variable.  It could be configured to use the length parameter as its base quantity, resulting in a 10' section listing a quantity of 10', rather than a quantity of 1 piece.  Or you could leave its quantity as a count, and embed the length in the Description field.  There are probably a lot of other possibilities, it just depends on what you need.

[Curtis_Waguespack]

Hi k-dawg,

Thanks for supporting the book first of all. As for your questions on setting this all up, it looks like you're on the right path.

The workflow I was going to suggest that you explore, is the use of multi-body part files for templates.

For instance, I've attached a door that has been modeled as a part file, with the rails, stiles and panel being separate solid bodies. This file would be the template for all of the doors of this style, and would be saved in your template directory. Then when you wanted to create a new size you'd start with this door template, change the overall size and then use the Make Components tool to save out the solid bodies as individual parts, and have them placed into an assembly. The parts in the assembly are grounded in place, but can be ungrounded and constrained if needed.

When you use the Make Components tool you can specify the template to be used in creating the new files. If you specify a template that is pre-configured to include the iProperties and property expressions as jtylerbc has suggested, you should be able to get most of the information you want to see in the final drawing to drop out automatically.

This all akin to the skeletal modeling workflow that many use (and might be another thing to look into. Here are a couple of videos showing the multi-body and make components workflow:

http://youtu.be/11dyV4InbmI

http://youtu.be/iDRotf2Is2g

This is all just food for thought, you might find that it isn't the correct workflow for you, but it might give you some ideas. I had hoped to steal away a few spare minutes to work though this door example, but I'm not going to have the time to do so. This file is an older file that I just updated quickly, but hopefully it'll give you some ideas. When you save this file, there is some iLogic that prompts you to change the size, etc.

Even if you find that the multi-body and make components workflow, is not for you, I think you'll find iLogic to be part of your solution at some point.

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

[Anonymous]

Thank you again Curtis and jtylerbc. You don't know how many times I have re-read what you typed. I watched the videos you posted and a few more from AU and it's making much better sense now. I would have to agree....multi body parts and make components look like the direction I was heading anyway, with iLogic not too far behind. It makes the most sense to me ATM.

One thing I was having trouble with is all of the constraining and assembling when getting to the assembly file. I think that most of this is now taken care of with the multi body parts. Essentially, I am making the large casework as one part, so a full, mid sized kitchen would be around 8 parts total. 

For a crude solution on the moulding, I have a few of my crown profiles ready and extrude along a path with parameters in a part file that actually punch out what I need. I constrain in the assembly with 2 or 3 clicks, but I'm guessing that there is a much better way. Modeling it onto the part (cabinet) I don't think will work since I will have inside and outside miters to deal with. It probably would work somehow, but I'm not sure that is quite as intuitive to me.

I still haven't looked much into the property expressions but it does seem that is also part of my solution. 

The Inventor user I have been watching with the iLogic for cabinetry is Mark Randa. Not sure if you have seen his video's but this is what inspired me the most to take the leap with INventor. I'm certain that iLogic is the right direction.

http://www.youtube.com/watch?v=bBpN7Ex4jJE

If I take the time and make all of these full cabinet parts, will they be usable in iLogic?