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Inventor BOM template for wood working.

13 REPLIES 13
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Message 1 of 14
moldydogpoo
4003 Views, 13 Replies

Inventor BOM template for wood working.

I am new to these forums and would have a question at which I need help with. I am trying to get my BOM to have length, width, and thickness of the parts. I am working with casework and mill work for woodworking. I am trying to get a template set up so i can have this automatically set it self when I pull it up in the idw file. 

If anyone can please help me that would be great!!! I am trying to get everything going and this is something that I really need to figure out. I can do all the clicking and that stuff, but if you have a working template or something that you would not mind sharing that would be awesome!! I will take what I can get. 

Thanks,

Moldy

13 REPLIES 13
Message 2 of 14
mpatchus
in reply to: moldydogpoo

All you really need to do is include Height, Length and Thickness as Parameters in your parts.

Have those parameters mapped in your assembly and utilizte them  in your idw Parts List.

Woodworking.JPG

I've included the rough templates I created.  You will have to tweak them to suit your requirements.

 

Mike Patchus - Lancaster SC

Inventor 2025 Beta


Alienware m17, Intel(R) Core(TM) i9-10980HK CPU @ 2.40GHz 3.10 GHz, Win 11, 64gb RAM, NVIDIA GeForce RTX 2080 Super

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Message 3 of 14
moldydogpoo
in reply to: mpatchus

Thank you for the basic template. I was wondering if you could explain to me how I can do this from scratch myself. I am trying to figure this out so when ever i start drawing a new part it automatically places the length width and thickness in the BOM list. I am trying to figure this out and would like to know. 

Thanks,

Moldy

Message 4 of 14
mcgyvr
in reply to: moldydogpoo

This should cover it

http://www.youtube.com/watch?v=luViJMQf3EI

 



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Inventor 2023 - Dell Precision 5570

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Message 5 of 14
laura.gilmore12
in reply to: mpatchus

How would this work for a multibody part with solid bodies in the same part file having different lengths, widths and thickness?

 

Thanks,

Laura

Message 6 of 14
mslosar
in reply to: laura.gilmore12

You can also write it so that all your parts have parameters set for length, width, and height and simply make that your description.

 

In the parameters window, you can rename the parameters you want to LENGTH, WIDTH, HEIGHT, or simply add them as three new parameters and set them equal to d1, d7, and d74 or whatever values are there. Then, click the box to Export those parameters.

 

Then, in the description of your part you can name it:  =STUD <LENGTH> X <WIDTH> X <HEIGHT>

 

Which, when displayed will look like 2" X 4" X 72".

 

 

Message 7 of 14


@laura.gilmore12 wrote:

How would this work for a multibody part with solid bodies in the same part file having different lengths, widths and thickness?

 


Hi laura.gilmore12,

 

The solids will not show in a parts list as separate lines. To do that you need to use the Make Components tool to write out all or some of the solids to the assembly as separate part files, and then:

 

    A) edit the derived base part in each file to link the parameters from the "master" file into each individual part

  or

    B) use some automation at the assembly level to get the L, W, T for each part, based on the bounding box, and

        push it to custom parameters/iProperties in those parts, so the BOM has information to report on the dimensions of each piece.

 

I think most people that are doing this type of work with multi-body workflow choose B.

 

An example iLogic rule to do this is at this link:

https://forums.autodesk.com/t5/inventor-forum/separate-multibody-part-inside-assembly/m-p/7171674#M6...

 

 

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

 

 

Message 8 of 14

Thank you Curtis,

I am working through your post and file from yesterday and trying to produce a simplified sketch using iLogic. 

I didn't want to repeat a thread if it has already been addressed, but as you suggested, probably makes sense to start a new thread on workflows for built-in cases and cabinets.  

 

Thanks,

Laura

Message 9 of 14

Curtis,

For path B, can you explain what you mean a little more in-depth regarding "use some automation at the assembly level to get the L, W, T for each part, based on the bounding box" or are you aware of a tutorial that would help me understand?  

 

Thanks,

L

Message 10 of 14

Hi laura.gilmore12,

 

See this quick video, that shows the basic steps. I pasted in the code from the other thread. Also, note that there were a bunch of extra iproperties in the part file. That was just due to my custom template that the Make Components tool grabbed by default, the ilogic code only creates 3 custom iproperties Length Width Thickness.

 

At the end of the video I showed adding the custom iproperties to the BOM using the custom iProperties chooser (or whatever that button is called), but most likely you'll end up wanting to do this in your parts list style , so the custom iprops are there by default, and so you can set up that parts list style to sum values and create cut list, etc. if needed.

 

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

Message 11 of 14

Curtis,

Thank you, this was helpful.  I guess you would have to continue to add logic to adapt for grain direction which would impact length and width for sheet optimization.  I know there are third party programs out there (Woodwork) that do this and I can see their value if I was doing this for every project.  

I have spent a lot of time over the last few days trying to develop a parametric shelving unit, unsuccessfully. This seems to get really tricky and breaks at the patterning level when you get into placing grooves and rabbets for joinery or adjustable shelving.  I will have to post on that.  

 

As a far as the next step once I have derived each unique component into the assembly file, it seems like I then have to reassemble the repeating components and these will no longer be tied to the geometry of the base model like those that have been derived.  

 

Thanks again for you assistance on this. 

Message 12 of 14
jtylerbc
in reply to: laura.gilmore12


@laura.gilmore12 wrote:

 

As a far as the next step once I have derived each unique component into the assembly file, it seems like I then have to reassemble the repeating components and these will no longer be tied to the geometry of the base model like those that have been derived.  

 


I do a lot of multibody work for welded plate steel fabrication, and there are some similarities to what you're trying to do with wood.  You are partially correct here - you do have to manually assemble the repeating components.

 

However, if you have your layout part (what you referred to as "base model") in the assembly, you can constrain the repeated components directly to the corresponding faces on the layout part.  This is almost as stable as the automatically placed and grounded initial parts, though obviously it is some additional work for you.

Message 13 of 14

Hi laura.gilmore12,

 

re: Grain Direction
There are a couple of approaches for this, but I would think some code (iLogic) would be the tool for doing it.

 

re: Joinery

I prefer to have these things be "feature based" rather than "sketch based", so basically the joints are based on the 3D not the 2D. In the model I posted on the other thread, I used Combine features to subtract the shelf from the side. There are other methods that could be used, but I think the feature based approach will eliminate most of the issues you're seeing.

 

 re: Replacing Repeated Components

You don't really have to do this. You could output all of the multi-bodies using the Make Components tool, but you'd end up with duplicate size part files on disk. The BOM will count them as the same part if they have the same Part Number iProperty, so you can use the BOM editor to make these same part files have the same part numbers manually, or we could use some code to set the part number based on the size. My preference is not to have duplicate files on disk, for the same part (part number). But there are tools in Inventor that create multiple files for the same part, so maybe it's not that big of a deal. The tools to make either approach work are available.

 

In your first posting, I mentioned this topic would "grow legs", and it's all of these questions that I was referring to. It can all be done though.

 

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

 

Message 14 of 14
Anonymous
in reply to: moldydogpoo

Hi,

 

Have you try that ?

https://www.woodworkforinventor.com/ 

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