Sheet Metal Gauge in Drawing

[kellings]

I have created a bunch of sheet metal rules for my different gauge thicknesses. Is there a way I can propogate the gauge information to my drawing so that if I were to change the gauge, that info would also update on my drawing sheet? The only thing I can get to work currently is to pull in the material used, but that doesn't include the gauge.

Any help would be appreciated.

[nmunro]

Create a custom property in the sheet metal part. Enter =<Sheet Metal Rule> as the property expression.

In the drawing the custom property value can be used in Text, title block property, parts list, sketched symbol, etc.

Of course, this will be the full rule name, not just the gauge.

[tdrawdy]

I have a few files you can edit to fit what you need.  Send me an e-mail address and I can forward them to you.

[SeanFarr]

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@nmunro wrote:

Create a custom property in the sheet metal part. Enter =<Sheet Metal Rule> as the property expression.

In the drawing the custom property value can be used in Text, title block property, parts list, sketched symbol, etc.

Of course, this will be the full rule name, not just the gauge.

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Can some expand on this? I don't quite understand, If I name my sheet metal rules appropriately, I could get rid of the material iproperty in my title block which only shows the material and not thickness...just not sure how to set this up, create the custom iproperty in the sheet metal part, then I can call out the iproperty in my title block??

I found this in the help:Use Sheet Metal Rule as Text Parameter

I run into issues with step 9, it says select custom properties - model, I don't have this option in the drop down...

Thanks

[mrattray]

Do you have a view of that part you created the property in placed on the sheet? Are you editing the title block in context of the sheet or in context of the drawing (in other words, did you expand the sheet and right click on that title block or did you right click edit from the drawings resources node?)

[SeanFarr]

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@mrattray wrote:
Do you have a view of that part you created the property in placed on the sheet?

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I added this "sheet metal rule" as a custom parameter to my template file and re-saved the template file, no part created...

My attempt was to add the custom parameter to my sheet metal template,

then add text parameter in my title block and call it out in every drawing...

the wiki help says there should be a custom properties - model in the type drop down...i don't see it...

Thanks

[mrattray]

The model properties are only available if you place a view of a part onto the sheet. You need to make a temporary part from your template with just a random extrusion or whatever in it, and place a view of it into your template. Then you'll be able to access the custom properties from the drop down. You can then delete the part from the drawing template after you've set up your title block and re-save your drawing template.

[swhite]

You can make any field show whatever parameter you have set as well. An example is our plates. We have the description column set as "=PL <G_T> x <G_W>" This automatically adds the thickness and width to the field. You could do something similar with the guage, just use <> to enclose your parameter name.

[jingyi.liu]

Hi Sean

Have you placed one view on your drawing? if you placed but still didn't see the property, I  guess you created a custome property in your drawing file other than the sheetmetal part file.

Regards,

[SeanFarr]

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@jingyi.liu wrote:

Hi Sean

Have you placed one view on your drawing? if you placed but still didn't see the property, I  guess you created a custome property in your drawing file other than the sheetmetal part file.

Regards,

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I didn't create the custom property in the drawing file, if fact I followed the tutorial to a "T", haha

I think there should be one line added to the turorial, (some of us might not know that adding at least one view is required)

Thanks!

however after placing one view on drawing sheet this is the result i get, instead of the sheet metal rule being displayed, i get...

[mrattray]

Did you miss the "="?

[SeanFarr]

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@mrattray wrote:
Did you miss the "="?

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Hey Mike, for some reason the = sign goes away once I press apply, I entered it in correctly, even copied and pasted it in there, but it disappears?

possibly a bug??

[SeanFarr]

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@SWhite wrote:

You can make any field show whatever parameter you have set as well. An example is our plates. We have the description column set as "=PL <G_T> x <G_W>" This automatically adds the thickness and width to the field. You could do something similar with the guage, just use <> to enclose your parameter name.

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Where and how to you find or come up with G_T pr G_W? or how does one know the <Sheet Metal Rule> will actually pull the sheet metal rule out into a text box from the sheet metal part file?

I am slowing digging into iLogic and automating a lot of steps that are manually done. I have lots of ideas, but searching around for something that you do not know the name of makes it hard. is there somewhere within inventor that these names are stored?

[mrattray]

This is nothing to do with iLogic, this is just pulling properties into other properties. It's a standard Inventor function as old as sand. I'll play with this in 2014 for you when I get a break in my work.

[SeanFarr]

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@mrattray wrote:
This is nothing to do with iLogic, this is just pulling properties into other properties.

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I understand this, for this particular issue, yea it is just pulling data from a table and inserting it.

going back to message 8 from steven, he states that G_W will produce the width value and G_T will produce thickness and I'm going on a whim here, but G_L will produce length? how does one come about these parameters? is there a document or location where it lists these parameters and what they hold for data?

Thanks Mike for looking into this...seems to easy to not be working??

[mrattray]

I think those are parameters Steven created in his parts.

[swhite]

my G_W, G_T and G_L are just custom fields we have put in our part templates in our parameters for Width, Thickness and Length. As long as you have a parameter that contains your rule, any field can be used to display that parameter.

Once you hit apply your "=" sign should dissapear untill you click back into the field.

Attached is a sample of our basic plate template. Whatever value G_L is set for becomes the length, etc.

Hover your cursor over the highlighted field in the part and you will see the example. Simply by changing the parameters, the part will resize accordingly. I could also type G_L=10 into my sketch as i was dimensioning it for those that don't have this parameter preset. So you know our basic part template creates a plate 10 x 10 x 1 to which we resize accordingly. We do not start out with a blank sketch, but have made an actual plate and saved that as our template so we coulod assign G_L etc to dimension values.

Even though content center parts use BL for length, we put a custom field "G_L" in all of them because with FG BL does not always equal the true length on multiple end angle trims. On those rare equations it differs we put in a sketch and assign that value to G_L, which defaults to BL at start.

[SeanFarr]

Ok, so after opening your template, your G_L, G_W etc are actual parameters that you renamed in the parameter dialog menu.

In the drawing enviroment, these values are pulled using those parameters.

So now, applying that logic (not iLogic) shouldn't there be somewhere in the parameters dialog menu defining the sheet metal rule??

Also i noticed that you have export parameter checked out, this seems to let the parameter be used in the drawing??

[SeanFarr]

Before this gets too complicated maybe I should state what I am trying to accomplish.

My title block contains a material field. I have 2 iproperties that populate this field,

one is material and one is comments, both from model properties. The material is typically Steel, Mild and the comments section I fill out based on material used, eg, 1/8" Sheet Metal or 1/2"x2" FB (Flat Bar)

I was hoping to automate the comments property by adding a third field that would be filled by sheet metal rule, which contains both material and gage or thickness. but it does not want to co-operate.

So if I create a sheet metal part, the material field in my title block would populate from the sheet metal rule property

and if i create a standard part, the material field would populate from the material and comments properties.

Unless there is a more efficient way to do this??

Steven do you use this template you attached for sheet metal?

[swhite]

Sheet metal parts add extra paramaters, one is Thickness which comes from the Sheet metal defaults.

This is a plate template but you could use Inventors default sheet metal template, make a sketch, assign parameters to dimensions and use the same basic premise, saving it back to a template. Thgen each one will fill out its own preset values.

Yes, they are set to export so they can be pulled into the BOM.

You could then set a field as such "= <Thickness> Sheet Metal" for the sheet metal and "=<G_T> x <G_W>  FB (Flat Bar)" for bar steel etc.

And yes, you could write a rule to grab these parameters and based on thickness put in sheet metal or flat bar, etc, but I'm not the one to ask about coding 🙂