Using model dimensions to fill "LENGTH/WIDTH" fileds in drawing parts list

[ironcleek]

In our “Parts list” (or BOM as we call it) on our .idw’s we have field for “LENGTH”. For example, we use round tubing. We would list the cut length of that piece of tube in the “LENGTH” column. As it stands now, we add “LENGTH” as a custom iproperty in the .ipt. Then in the drawing we add that property to the parts list to capture the length. This works fine, but I’m wondering if we can eliminate some steps by capturing the actual dimension from the sketch to automatically populate the “LENGTH” value. Needless to say, this would eliminate room for error (less typing) and will update the value automatically if length is changed or if the part is copied. I suppose the same would apply for “WIDTH” on sheet metal parts... How do I do this? Thanks for your input and help!

[jtylerbc]

ironcleek,

What you're looking for is indeed possible - in fact, almost every part I work on uses it to some degree or other.

First, you need to name your dimensions that need to be used in this manner.  You can do this by a few different methods (Parameters box, Dimension Properties), but my personal favorite is typing it into the value entry box.  For example, if you have a plate with a width dimension of 5", instead of just typing "5" in the box, you'd type "Width = 5".

Next, you have to mark those dimensions for export.  Exporting essentially just creates a custom iProperty that automatically gets its value from the model parameter.  Go to the Parameters dialog box, and check the boxes in the Export column for the relevant values.

Then you may want to format the properties a certain way (units, fraction/decimal, precision, etc).  Right click on the parameter in the Parameters dialog box, choose Custom Property Format, and set the options as desired.  Note that there's a checkbox at the bottom to copy the settings to other similar parameters - this can save you some work if they're all intended to be the same.

You can then treat your parts list exactly the way you already were for your custom LENGTH property, except it will be picking values up directly from the model. 

Additionally, you can embed the dimension properties into other iProperties, by enclosing their names in <> and forming an iProperty expression.  For example, in the description of a 5" x 10" plate, you could enter:

=PLATE <WIDTH> X <LENGTH>

There are some addtional tricks you can pull using sheet metal extents specifically for sheet metal parts, but I'm just starting to look into those (we don't use much sheet metal), so I'll leave that to someone more experienced with it.  Hopefully this will be enough to get you started.

[Cadmanto]

What I am thinking to address part of your issue is, in the out of the box versino of Inventor there is

a parts list called "Parts List (ANSI)" when we used frame generator the CC structural parts came in as cut lengths.

Maybe create your own custom parts list using this one as a benchmark and rename the column header to be "Length".

[ironcleek]

Outstanding! I thought there was a way. Thank you for your help.

[SoulAsasin]

Hi everyone.

This method works great if you know the size of your part form the start. The problem is that I often create complex unic parts, and after I am finish I always have to measure the size of my biggest dimensions and enter the values manually. I could use the above method and if I want to modify the dimensions of my part, I should only change those parameters that set my stock number and then cut the material that I don't need, like in real life milling. But somethimes I am in a hurry (because my company decided I needed to be 🙂 ) and is much faster to just ad some material in a part or another. Then the above method doesn't work. Can Inventor somehow calculate my biggest dimensions on X Y and Z direction? I know it can, because when you press the home view it always zooms so the enire part can be visible. I just don't know how to get that info into my stock number parameter.

Anybody any ideea on this?

[jtylerbc]

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@SoulAsasin wrote:

Hi everyone.

Can Inventor somehow calculate my biggest dimensions on X Y and Z direction? I know it can, because when you press the home view it always zooms so the enire part can be visible. I just don't know how to get that info into my stock number parameter.

Anybody any ideea on this?

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Yes.  We use an iLogic rule that works on that principle, used for getting the extents of plate steel.  If you're familiar with iLogic, look into the ExtentsLength, ExtentsWidth, and ExtentsHeight functions (listed under the Measure category of the snippets).

Once you have a rule that measures those distances, you'll want to set it up to transfer those measurements to an iProperty, or a User Parameter.  I typically use a User Parameter, because you can then use the Custom Property Format settings I mentioned in my previous post to control the appearance of the iProperty.

[jeremy_wasserstrass]

In that case add User Parameters for length and width and mark them for export. When you are finished with the part link those to the parameters that make up the length and width of the part. This will also allow for multiple parameters to be added together to get a total length or width. Another option I have heard of someone using is to start every part as a sheet metal part. This allows one to use the sheet metal extents to get width and length, the only thing to be aware of there is that the output of the sheet metal extents is always in mm and there is no way that I know of to change that in Iproperites or parts list.

[Namoi1]

In frame generator the length is G_L and is automatically generated in User Parameters. 

What I've done upto now is my standard parts list style with a column Lg that looks for a iproperty Length.  My standard part template is saved with a user parameter Length which is exported, that way I don't have to format it all the time and it's easy to say Length = d10 for example which could be driven.  I might use that Ilogic rule though sounds really good.

What I want to know is that if I change the User Parameter exported in my template to G_L will this stuff up the frame generated parts?  If not I'll change the parts list to use G_L instead of Length and all my parts will be similar for the parts list.

[SoulAsasin]

Hey

Thanks alot.

This is exactly what I was looking for. I will give it a go.

[jtylerbc]

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@Namoi1 wrote:

What I want to know is that if I change the User Parameter exported in my template to G_L will this stuff up the frame generated parts?  If not I'll change the parts list to use G_L instead of Length and all my parts will be similar for the parts list.

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If I'm following you correctly, no, that' shouldn't cause any problems for the frame generator parts.  However, it may not be necessary.

In the parts list, you can apply Substitution to a column.  In your case, you could create the parts list showing a column for Length, and add a substitution of "G_L" to it.  If it is a part where the G_L property exists (frame generated), it will use that value.  Otherwise it will just show the Length property like usual.

[mbrightonNPXL8]

I realize this is a very old thread, but can you clarify exactly how to go about doing this? We use Assembly Models in 2021 and are looking for a way to get LWH of all the ipts (which are mostly square Blocks of Aluminum/Steel/Plastic) to pull into the BOM so we can export an Excel Document and use it to order materials.

[mbrightonNPXL8]

Sorry this was in response to the overall XYZ Measurements since we also use thicken/extrude to adjust block sizes often and cant rely on original dimensions for block sizes.

[SharkDesign]

This is the method mentioned above

https://youtu.be/aPn7QBzYzDg

You can also directly access parameters from the text box itself and they auto update. 

If you want to measure bounding boxes which it sounds like you might do, you're into iLogic territory.

[johnsonshiue]

Hi Matt,

This is doable with a simple iLogic rule (see below link).

https://forums.autodesk.com/t5/inventor-forum/help-iproperty-populate-ilogic/td-p/3940420

The reason why iLogic is needed here is because the body extents are not automatically captured as iProperties. You need to use Inventor API to access those properties and populate them to iProperties.

Many thanks!