Please help a noob with creating a parts list with length, width and thickness

[ehayes1293]

Hi, 

My name is Eric and I'm a noob.

I've been trying to learn Inventor so I can get into woodworking as a hobby.  I been spending a lot of time developing a workbench as a first project.  I think I have it ready to build, and was hoping I could print out the part list with dimensions to see how much wood I need to buy (i.e. how many 8ft 2x4, and how much 3/4"  plywood.  I had a created a bunch of user parameters to help me build it and if needed, quickly adjust some dimensions which would change everything.   (i.e  I have Table_Length, Table_Width, Frame_Thickness and Frame Width (Setup for 2x4, but could change to 1x4 if I want).    I was hoping that I could generate a list of all my solid body parts with Length/Width/Thickness listed for each.  I don't see that option and I don't know how to get it.     

So in case you need the info, I sketched each part in the same part file, extruded each as a separate solid body, then used the Make components feature to create a .iam file with all the various solid bodies.

I've tried googling and looking at YouTube, but I cant's seem to figure it out. However, I have seen some videos where the user showed a part list on the drawing file view with a separate column for L, W, Thickness. 

Thanks for any help you can provide

Eric

[mdavis22569]

Here are a couple of examples I have of templates that might give you some idea's 

These have custom iproperties that have L / W / H ...and populate in the Description ...which populates in the parts list 

Is this what you're looking for?

[ehayes1293]

thank you for the quick reply!  So, would I have to go into each of my solid body parts and edit the iproperties for each?

regards

eric

[mdavis22569]

You would do it in the parameters ...

You could link it to a common Excel spreadsheet and populate the values

Or you can pre-populate it 

[kelly.young]

Getting familiar with parametric modeling and Frame Generator would be a great way to get your woodworking future started.

Frame Generator Tutorial

You can read through this older Forum post, it goes through advanced techniques. From the way you are describing things you might be able to get some good ideas through a few of these links, although many are fairly difficult or outdated. If you have files you want to share we might be able to get you started in the right direction.

Challenging Woodworking Tutorial

[chris]

Just create a set of templates that already have the formula's in the description feilds

[john_s2]

Hi Eric,

This is both relatively easy and relatively complicated subject to how you have created your bench.

If the bench is an assembly of individual Parts you need to go to each part file and change the appropriate driving parameters from d1, d2 or what ever to Lth,  Wth and Thk  or however you want to define Length, Width and Thickness (I use LENGTH, WIDTH & THICKNESS as names) you need to be consistent throughout so all the parts are exactly the same.

You also need to tick the Export Parameter box for each of these renamed parameters

In your drawing for the assembly create a Bill of Materials and edit it using column chooser. It is most probable that Lth, Wth and Thk aren't available in the lists of possible columns so you will need to create these as new parameters so to add as columns.

That is pretty much the gist of it from an assembly of individually generated parts or iParts - for iParts you will have driven the different sizes based on Lth Wth and Thk parameters.

If you have generated the bench as a single part as a multibody solid, you then need to extracted them, as individual parts into and assembly. You then need to run an iLogic rule to measure each part and define the Length Width and Thickness for each part individually.

The Rule I wrote to achieve this is:-

'MEASURE PANEL DIMS'

'Measure The object and create variables

L1 = Measure.ExtentsLength
L2 = Measure.ExtentsWidth
L3 = Measure.ExtentsHeight

'Sort measurements

THK = MinOfMany(L1,L2,L3)
LTH = MaxOfMany(L1,L2,L3)
WTH = L1 + L2 + L3 - THK - LTH

'Create external custom parameters

iProperties.Value("custom","LENGTH") = LTH
iProperties.Value("custom","WIDTH") = WTH
iProperties.Value("custom","THICKNESS") = THK

Note that I use LENGTH  WIDTH and THICKNESS as the custom column parameter names in BOM columns. 

[Anonymous]

Hi

There is an easy solution for your problem, at the assembly environment , click below the description column beside the part you wish to add the dimensions to it and just write it, click done, and you'll have it in your parts list.

I f you don't have the Column, you just right click on any column there and select run time column customization , all Column will be displayed, select the desired keep click and drop it beside any of the existing column you wish ...

Hope pics down will help

for further question and tutorials I'll be glad you visit to my channel on you tube

https://www.youtube.com/results?search_query=ebrahim6000

have a nice day

Eng.Ebrahim

Hope it's clear

[mdavis22569]

Did you try one on my settings?

[ehayes1293]

Thanks for all the suggestions.  I haven't had a chance to try them out.  I was thinking maybe if I created template parts for all the types of wood I would use give them all the same parameter names (Length, Width, Thickness) and then just basically load them into an assembly file and edit and assemble them, that would maybe work. for example I d' have the following part files:

2x4.ipt  with Parameters (Length, Width, Thickness)  - Would just use a 8ft x 3.5"x1.5

.50 Plywood Sheet with same Parameters (Length, Width, Thickness) 8ft x 4ft x.5"

etc

I was hoping I could bring these standard materials in to a file, and then modify them to correct dimensions.  However, I realized when I did that, it changes all the same parts.. For example, I brought in 4- 2x4 parts.  But wanted to make them different lengths then the original.  If I change one (editing Parameters), they all change.  I was hoping to just bring in the  template part as many times as I want, then save each as new part for the specific project (i.e. Leg 1, Leg 2, etc) with editable parameters that are not linked to each other.  Not sure that is best practice or even doable.  I did read something where somebody used iLogic to prompt when a new board was added to edit the dimensions.  That would be ideal, but would it still change the original template file and thus give me the same issue?

Thanks for any help

Eric

[swalton]

Try putting your 2x4 part in your template directory and starting your next dimensional lumber part from that file, rather than standard.ipt.

If I did a large amount of work with dimension lumber and sheet goods, I would make custom content for Frame Generator or the Content Center.

See

https://knowledge.autodesk.com/support/inventor-products/learn-explore/caas/sfdcarticles/sfdcarticle...

or

https://knowledge.autodesk.com/search-result/caas/CloudHelp/cloudhelp/2017/ENU/Inventor-Help/files/G...

[kelly.young]

Hello @ehayes1293 how is your woodworking going? Did you ever get a chance to implement any of the suggestions?

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

[Tradnu]

Hi John,

I successfully followed your ilogic rule solution for generating LTH, WTH, THK parameters for multibody solid (thanks heaps).

I'm hoping you might be able to answer two further questions along similar lines:

1. Is it possible to concatenate those values WTH, LTH, THK into a new custom column parameter i.e. CutSize so that it displays the following: Lth value, space, 'x', space, WTH value, space, 'x', space THK value, units?                   For example (50 x 80 x 5mm)
2. Is it possible for your iLogic rule to be applied to all future multibody parts without copying your rule into every new part I create?  If so, what configuration/changes would I need to make?

Thanks for taking the time to consider my questions.

Warm regards 🙂

Undart

[johnsonshiue]

Hi! I believe both are doable. The concatenation can be done by using iLogic or VB.Net's string functions. In terms of populating a rule, the quickest way is to make it an external rule and set up an External Rule folder (Tools -> App Options -> expand the panel -> iLogic Options).

Many thanks!

[dolanR3U6S]

Great info on this thread, I found it searching for a way to do something very similar.  I make cabinetry and custom millwork using multi-body part modeling, so all the options for this programming that involve settings within the individual .ipt file don't really work right since all the defining dimensions and data are in the source .ipt file (parameter names, dimension d values, etc.).

So with this last post, I am also interested in setting up something so that when I create each individual .ipt file from a multi-body part, I don't have to run a rule (or more likely forget to run a rule).  So please clarify how the external rules work, with the external rule folder... I am not sure how to do that.

Thanks!

[johnsonshiue]

Hi! It is better to post an example and describe what you want to do with it. The forum experts can help take a look and provide further guidance. This particular request should be doable using an iLogic rule.

Many thanks!

[majnalt]

Undart, where does your length, width, thick information store in multi body part upon running the rule? 

[chris]

@ehayes1293 Are you trying to maintain the length, width, and height manually or have it automatically populated?