Auto Cut-list for LENGTH, WIDTH, THICKNESS – Possible?

[OliverTilbury]

Hi all,

Could someone please point me in the right direction (or directions!) for generating a Parts List with columns for LENGTH, WIDTH and THICKNESS which are auto populated with values from the parts?

* While writing this post I have come across some other forum threads and the most useful of which  (in my view) I have pasted the links to bellow. 

I'll still post this thread  however in case there is any more guidance out there on top of or in conjunction to those threads (in particular the iLogic they suggest as this seems to be the most likely route of enquiry ). Thank you. 

Use example of us:

I have a piece of timber joinery of an MDF or Plywood frame made up of numerous panels of varying shapes and sizes.

This has been made as a multi body part (because that must be the most robust way to do it given there is a lots of chopping and changing as the design progresses).

 

I have then turned this into separate parts in a new assembly by selecting … Manage > Make Components.

So now I can at least generate a Parts List for all the panels!

What I would now like is some efficient work flow to capture those extents dimension and pull them into the Parts List. Pressing a buttons to auto generate your cut list would be the Holy Grail!! 😊

One caveat / work flow I don’t want:

I have seen from searching online some talk about creating reference dimensions, naming them LENGTH, WIDTH, THICKNESS so as to become Custom Parameters, checking the parameters for export and then setting the column in the Parts List to look for said parameters.

However that is surely extra manual work!

I would sooner take the dimensions from my 2D drawings (of the assembly - which I have to do anyway!) and manually generate the cut list in Excel rather than this extra time consuming step of creating reference dims, parameters for each and every extents dimension in every part.

If there are hundreds of unique panels this could take ages!

Also in my line of work (bespoke furniture) there is no future benefit to generating fancy links/references (as the furniture will not change that much once it gets to the cut-lis stage) so you're better off doing it manually if a quick auto way does not exist. 

Couple of useful related threads: 

https://forums.autodesk.com/t5/inventor-forum/using-model-dimensions-to-fill-quot-length-width-quot-...

Main take-home from this is the reference / user parameters route. Although  @jtylerbc  mentions a tantalising iLogic rule??

https://forums.autodesk.com/t5/inventor-forum/part-minimum-dimensions-iproperties/td-p/7505524

This has an interesting iLogic rule by @Curtis_Waguespack that in his words "Then in the resulting assembly [produced from a 'master' multi-body part] I would create an iLogic rule and paste in the code below and run the rule, which will step into each part

 and write custom iproperties for the length width and thickness of each part."

This could be what I am looking for although apparently the only limitation of this code is that if a part is on the skew to the xyz plane then it will take the max dimensions but still in the xyz rather than true to the face of the panel. But to be honest in most cases for myself, most panels will be at 90 degrees to each other (i.e. along xyz) so that will probably be fine 'in most cases'. 

Any further thoughts / advice?

Thank you.

[MechMachineMan]

The most fool proof way I've seen is to create template parts for a generic flat plane, with Length, Width and Thickness already modelled in on the sketch. These values are then put into a form for whenever you create a part from that template.

Workflow.

0. Create and config template.

1. Click on template file to create part.

2. Enter L, W, T values in the pop-up form and watch it auto-generate a "blank"

3. Continue modelling using a "subtractive-modelling only" method (ie; prevent users from adding extra material outside of the established LWT)

4. Watch it all beautifully auto-populate and be controlled, AT THE TIME OF DESIGN, by the user.

If you have done nothing like this beforehand, then you are likely looking toward unreliable results. If the geometry isn't aligned square to the origin planes, all of the L,W, T dimensions gathered through any iLogic or anything will be skewed, as they ONLY ever measure the extremes in an orthogonal means from the origin planes.

[jtylerbc]

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@MechMachineMan wrote:

If you have done nothing like this beforehand, then you are likely looking toward unreliable results. If the geometry isn't aligned square to the origin planes, all of the L,W, T dimensions gathered through any iLogic or anything will be skewed, as they ONLY ever measure the extremes in an orthogonal means from the origin planes.

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The iLogic method I described in the referenced thread technically has this issue.  We use the Direct Edit command on skewed parts like that to re-align them with the origin, then constrain those parts to the Layout part (instead of just Grounding them in place).  It's an extra step, but in actual practice it comes up so seldom that the extra step isn't really a problem.

Our work is a mix of individually-built parts and multisolid techniques, so that problem really only comes up in the multisolid scenario. 

[OliverTilbury]

Thanks for the comment.

Means can't use the multibody workflow. Although could work for stand alone / normal parts.

I do like the iLogic code that auto create iPropoties in the parts for length, width, thickness as long as the part is normal to the origin planes.

Although I need to try and tweak this code as seams to trip over if - for example - width and thickness are the same.

Change the IF statements I guess.

[johnsonshiue]

Hi Oliver,

I believe you can use Sheet Metal Multi-Solid Body and Multi-Thickness workflows to do this. After you are done, you can push the solids to individual parts and create flat pattern in each part. The length, width, and thickness can be captured on BOM table

Many thanks!

[MechMachineMan]

If you check out my signature, I actually wrote a macro earlier that can reorient the parts if they are skewed, using the API and the direct edit commands. Please read the thread for notes on it's usage. ( Link also here: https://forums.autodesk.com/t5/inventor-customization/ilogic-move-bodies/m-p/7786379/highlight/true#...)

If you have any issues with it, it would be cool if you let me know, so I can fix it.

So this reorient rule combined with the measuring macro could be pretty useful.

Good luck!

[PaulMunford]

Sheet metal extents was the easiest method I came across.

You might also want to look at WoodworkForInventor.

[jtylerbc]

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@Anonymous wrote:
Thanks for the comment.

Means can't use the multibody workflow. Although could work for stand alone / normal parts.

---

I use the iLogic method with multibody all the time.  Just have to watch out for those oddly oriented parts and correct for them, which isn't all that difficult to do.  Also, I would point out that I don't see any parts in your screenshot that would cause the problem in the first place, as none of them seem to be skewed relative to the origin planes.

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@Anonymous wrote:

Although I need to try and tweak this code as seams to trip over if - for example - width and thickness are the same.

Change the IF statements I guess.

---

I haven't seen your version of the measure code, so I don't know what your If/Then statements are doing.  My version doesn't contain any If / Then logic.  If you're using If / Then to try to identify Thickness, I may have a suggestion that could work better.

[jtylerbc]

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@MechMachineMan wrote:

If you check out my signature, I actually wrote a macro earlier that can reorient the parts if they are skewed, using the API and the direct edit commands. Please read the thread for notes on it's usage. ( Link also here: https://forums.autodesk.com/t5/inventor-customization/ilogic-move-bodies/m-p/7786379/highlight/true#...)

If you have any issues with it, it would be cool if you let me know, so I can fix it.

So this reorient rule combined with the measuring macro could be pretty useful.

Good luck!

---

I'll be checking that out as well.  Seeing as how I just got off the phone with one of our engineers helping him do it manually, while I was trying to write a reply to this thread where we were discussing it, I'd love to try out an easier way.

[OliverTilbury]

Thank you for the suggestion @johnsonshiue.

@PaulMunford I see this is also a suggestion you make. Could you elaboration on the exact workflow? I have mocked up a basic joinery cabinet (18mm MDF, 2 sides, top and bottom) and think I've turned into into a sheet meal part by (in the multi body part) clicking on the Environment tab then 'Convert to Sheet Metal'. But not sure what to do now.

Thank you. 

[OliverTilbury]

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@PaulMunford wrote:

You might also want to look at WoodworkForInventor.

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Yes I have come across WoodworkForInventor but imagine it is extra expense and would like to see what Inventor can do out the box before I have to pay for extra third party plug-ins. Not saying never is never though to such tools. 🙂

[OliverTilbury]

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@MechMachineMan wrote:

If you check out my signature, I actually wrote a macro earlier that can reorient the parts if they are skewed, using the API and the direct edit commands. Please read the thread for notes on it's usage. ( Link also here: https://forums.autodesk.com/t5/inventor-customization/ilogic-move-bodies/m-p/7786379/highlight/true#...)

If you have any issues with it, it would be cool if you let me know, so I can fix it.

So this reorient rule combined with the measuring macro could be pretty useful.

Good luck!

---

Thanks @MechMachineMan.

Before I give this a go can I just check a couple of things?... 

1) What is the difference between iLogic code and macros?! Sorry I am very much in the deep end here I know. Just want a cut-list  Although do want to learn iLogic and maybe VBA too as looks like give a lot of options once able to use. 

2) I have done a quick bit of reading about macros in Inventor and found this recourse 

http://help.autodesk.com/view/INVNTOR/2018/ENU/?guid=GUID-BDDB44A3-3415-44EB-B10E-216BB08BD614

It talks about macros either being "Inventor's VBA supports three types of projects: document, application, and user".

I also found this:

http://www.kwikmcad.com/icode/documents/macrodefault.html

Which talks about placing new macros / code in the Default.ivb as "This is a good place to stick things you always want available".

How / where would your recommend placing your code?

Thank you very much,

Oliver

[johnsonshiue]

Hi Oliver,

I assume these pieces are in different thickness values, right? If yes, you will need to create Sheet Metal Rule for each thickness value or material type. Go to Manage -> Styles Editor -> create a new rule based on existing one. Make sure the thickness value and material style are correct. After you set up the rules, you can go to the Solid Body folder in the browser and right-click on each solid body and make sure the correct rule is set.

Lastly, use Make Components command to push each solid as a part in an assembly. Open each part and create the flat pattern. The extents and thickness should be available as iProperties. Then they will show up in PartsList or BOM.

You may want to take a look at Neil Cross' video about the workflow.

https://www.youtube.com/watch?v=M3npmmadpO0

Many thanks!

[MechMachineMan]

iLogic is the basic "inventor customized" environment that has shortcuts in it, but runs on VB.net syntax.

Macros are accessed using the Macros tab in the tool bar. Macros can easily be added to buttons on the tool bar, or have keyboard shortcuts assigned to them - unlike iLogic rules. The macro environment requires A LITTLE MORE knowledge on programming, but comes with the IDE built into the program that makes it much, much easier to debug and test code.

VBA and VB.net are very, very similar, so if you learn one, you essentially know them both. There are a few differences in the libraries available and some of the syntax, but other than that, they are close enough. You can probably find lots of reading on converting between the 2 online elsewhere.

As far as placing the code, place it in the APPLICATION in a new MODULE, so it's accessible across all of your Inventor Documents. To run it, I would highly suggest investigating using keyboard shortcuts, or creating a button on the tab. If every other piece of customized programming you have is in the rule environment, it is also possible to convert it, OR to create a "Dummy Rule" which will in turn fire the VBA macro.

Let me know if you have any more questions.

Good luck!

[PaulMunford]

Sheet metal version runs like this:

1. Open your sheet metal template, create a 'Width' and 'Length' parameter.
2. Set your 'Length', 'Width' & 'Thickness' for Export, so that you can capture them in the BOM later.
3. Create an iLogic rule to map the sheet metal extents to your parameters (Code Below).
4. Set an event trigger to run the rule 'On any Parameter change'.
5. Close and save your template.
   Note: You could create multiple templates with Material and Thickness already defined.
6. When you export your bodies to parts specify your new custom Sheet metal template.
7. Don't forget to export any parameters you want to link to 'Thickness'.
8. Now you'll need to run through each component, opening it, triggering a sheet metal flat pattern, and (optionally) linking the thicknesses together
   (You can automate the triggering of flat patterns, check out the app store link below).
9. You can now reference your Length, Width & Thickness into your BOM. Should you update sizes, the BOM will update to your model and will be correct.

Try
	Length = SheetMetal.FlatExtentsLength
	Width = SheetMetal.FlatExtentsWidth
	Thickness = SheetMetal.FlatExtentsArea
	Catch
End Try

https://apps.autodesk.com/INVNTOR/en/List/Search?isAppSearch=True&searchboxstore=INVNTOR&facet=&coll...

[etaCAD]

Hi Oliver,

I'm close to finish a tool that gets the maximun size of parts, independet of their shape and orientation.

It is too early for publishing, but please check your PM for some preliminary details.

 Andreas

[NachoShaw]

I wouldn't accept woodworkforinventor as a solution for anything. I'm my experience:

It's too expensive
The support sucks (unless you enjoy sarcastic condescension)
Its too buggy
It's limited in customisation
It only truly works if everyone has it
It doesn't follow standard inventor methods

[OliverTilbury]

Hi all,

sorry for not responding for a while.

I have hit a very busy patch with work and probably going to need a week or two more before I can look into all these options properly and give it the time it needs.

In the mean time..

Thank you very much @johnsonshiue and @PaulMunford for your explanation of the sheet metal work flow.

 > One question for now though: does this work flow still require the solid bodies (as created within the resultant parts) to be normal to the origin planes... or would this creating flat pattern work flow handle bodies on the skew?

Thank you @MechMachineMan for the explanation on iLogic V macros. I will look into this and your macro solution. Thank you. 

Thank you @etaCAD for reaching out with the tool you are developing. This does sound very interesting. Yes I did get your PM and apologies for not replying as yet. A big job has come up that pays the bills and has had to take the driving seat!

Thank you @NachoShaw for your info on Woodwork for Inventor. That's interesting to hear an account from someone who has actually used it.

Thank you all. Will be back in week or so!

Oliver

[PaulMunford]

Hi @NachoShaw. When I first looked at W4I more than three years ago - I also wasn't impressed. However, V.7 and V.8 have shown massive improvements in functionality, stability and integration with Inventor. It might be worth you taking another look.

If you do - let me know what you think?

Paul

[PaulMunford]

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@OliverTilbury wrote:

 > One question for now though: does this work flow still require the solid bodies (as created within the resultant parts) to be normal to the origin planes... or would this creating flat pattern work flow handle bodies on the skew?

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Hi @OliverTilbury,

The sheet metal toolset creates an additional body within the resultant part file which is always normal to the design plane, so the Extents are always the Length, Width and Thickness of the part.

Does that help?

Paul