Sheet metal flat pattern width and length

[lcorrea876ST]

Hi,

I have inventor 2018 and I want to use the sheet metal length and width in my BOM, I have been reading that I have to put this in iProperties:

=<FLAT PATTERN LENGTH> cm

=<FLAT PATTERN WIDTH> cm

This displays the values in cm, it doesn't make any change if instead of typing "cm" I type "in"..

I red that this feature was just available in centimeters.. but it was posted in 2014.. I was wondering if this was fixed in 2018 version.

[doug.johnston]

You can change the units from the parameters browser by changing each one from cm to in.  I am using custom iproperties for extents_length & extents_width ..... 

Then I created a custom iproperty (CUT_SIZE) as a formula to display the overall length and width ... 

By doing it this way, my length and width always change based on the sheet metal size.

Hope this helps with your problem ...

Doug J.

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[Xun.Zhang]

Hello,

It was fixed in Inventor 2018 already, please follow the steps from Help document.

http://help.autodesk.com/view/INVNTOR/2018/ENU/?guid=GUID-9ED64200-A0CA-4F27-A308-9BF7ADB22D06

[lcorrea876ST]

It shows the dimension in decimal, I need it in fraction.

I can modify the format from decimal to fraction when the parameter is shown in the parameters list but in this case it won't show length width or area.. Is there a way to change the format?

[doug.johnston]

Can you post a picture of what you are getting and trying to do ??

I'm a little confused as to why you can't change the units.  Also, you might need to create a formula to get the area.

I assume you are using the flat pattern to get your values ... ???

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[lcorrea876ST]

As you can see in picture No. 1 I have a BOM, when I am using a standard part I can pull the material and length from the model using iProperties by clicking share parameter and changing the format from decimal to fractional(picture No. 2).

My original question was how to show the length and width of a sheet metal part in the BOM and it was answered.. I have to type "=<Sheet metal length> in iProperties (picture No. 3) but as you can see in picture No. 1 it it shared in decimal format.. In normal parts I can change the format from decimal to fraction in parameters but in case I am working with a sheet metal part I can't because the length and the width aren't in the parameters list (picture No. 4).

Bottom line.. I want to show in my BOM the length of my sheet metal part in fractions..

[johnsonshiue · Accepted solution]

Hi! If I understood your request correctly, this can be done using an iLogic rule and Custom Parameter Format. Please see attached part.

I created two user parameters: LENGTH and WIDTH and export them so they will appear in Custom iProperties. In the Parameters dialog, I changed the Custom Parameter Format to fraction. Next, I created a rule to capture the extent values. Lastly, the Custom iProperties form an expression to combine the two fractional values.

Please take a look and let me know if you have additional questions.

Many thanks!

[7021Httt]

Hi. Can you tell me how to use the Sheet Metal Length and Width and then have the possibility to remove precision and the units? This i did in Thickness in the paremeters/Custom Property Format see iProperties_3

[7021Httt]

Parts with iProperties.

[johnsonshiue]

Hi Henrik,

Here you go! I just added two user parameters (LENGTH and WIDTH), exported them, and set the proper format. Then I created a simple rule to equate the properties. Please take a look at the attached part and let me know if you have additional questions.

Many thanks!

[7021Httt]

Hi John. Just what i needed. Thanks for helping. 🙂 Henrik