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.

[Anonymous]

This is good, I will probably lean towards this method, as it seems useful for both standard and sheet metal parts...

I am still unsure why though the <Sheet metal Rule> parameter doesn't work, but anyway, there is always a solution.

Thanks for you time guys!

[mrattray]

I think there's an important distinction that needs to be made here. You cannot pull parameters into the title block, only properties. Checking the export box causes Inventor to automatically create a property with the same name and value as the parameter.
Where is your value for the current sheet metal rule coming from?

[Anonymous]

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@mrattray wrote:

Where is your value for the current sheet metal rule coming from?

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I manually type it in, in the comments property of the model's iproperties...which is why I was trying to use this **** <sheet metal rule> text parameter...so my idea was to make sure my sheet metal rules we named appropriately so that this info could be entered into my title block automatically, based on the selected sheet metal rule.

[Anonymous]

Just for clarification we never change the sketch that defines the plate lenght and width. To change the shape we attach a sketch to the face and define the end shape, so length and width are always correct.

So in your sheet metal template in the comment field put "<Thickness> SHEET METAL

just make sure Thickness is set for export.

[mrattray]

I meant how are you attempting to get it now?

[Anonymous]

In my sheet metal part, i created the custom i property as per instruction above

On my drawing sheet, I placed one view, inserted a text box, both on the drawing sheet itself and within the title block defintion, both return <Sheet Metal Rule> instead of the actual rule that was used in the sheet metal part which should be .75 Steel, Mild

Unless I am missing something?

I should add that I tried to use the custom iproperty with both Inventor 2013 and 2014

I am going to look into iLogic and see if I can spit something together to create a custom iproperty, grab the thickness from the sheet metal parts only and apply that to my title block along with material...

The thickness is not important for standard parts, I only like to include the material thickness in the title block for sheet metal parts because it saves drawing a view on the sheet to show thickness...

Thanks!

[Anonymous]

In your comment fiekld where you currently type it in, put =<Thickness> Sheet Metal

Make sure Thickness is set as export. In your text box go to Type > Properties - Model then under Property > Comments and click the Add Text parameter, let me know what you get.

[mrattray]

I just tested your exact work flow in 2013. (I'm multi tasking with a job that's in 2013, so I can't test 2014 at the moment) It worked fine for me. The only difference I noted was the value of the property as it appears in the property editor.

In my example I have a property named "test" whose value is “=<Sheet Metal Rule>” (copy/pasted from the link you provided earlier). The name of the active sheet metal rule in my part is "a0".

[Anonymous]

hmmm....maybe I have this wrong?

in my sheet metal template I have some sheet metal rules of different sizes.

Now I think this is where I am going wrong...I was under the assumption that I choose a rule from this list,

-create my part

-create the custom property with the =<Sheet Metal Rule> in the sheet metal part

-place a view on the drawing

-add tex box and populate it with the custom property - model and select the <sheet metal rule>

-I thought it would apply the rule I actually used, but I think it just applies what ever is in between the < >

If I set-up the custom property as this:

what shoud i expect to show up on my drawing? the actual sheet metal rule used within the sheet metal template or <Sheet Metal Rule>?

[Anonymous]

this works pretty good actually, only issue I can see is when selecting a gage, I would like that to appear if the sheet metal is an actual gage and not just a decimal...

That is why I was hoping to set up the sheet metal rules property, but I will take what I can get...

Thanks Steven!

[Anonymous]

You can right-click the parameter field and set the custom property format to display as a decimal or fraction, to whatever precision you want. You could set a iLogic rule inside the part to convert any entry similar to like

If Thickness = .1891 or whatever value

then Comments = 7 Guage, Mild Steel

else if Thickness = >.25

then comments = Thickness "Bar Steel"

End If

Not the proper format, you'll have to figure that out.

Did you type in <Sheet metal rule> or use the property insert?

[mrattray]

You should be getting the name of the rule actually used, Sean. It looks like you're doing everything right. I don't know what the problem you're having is, and unfortunately my work load just won't allow me to help you troubleshoot this. There's no reason to give up, though. This should be working like you expect.

[Anonymous]

I used the property insert for some reason the <Sheet Metal Rule> property is not working...

but your suggestions are definitely opening up some ideas...I will play around...might write a logic rule to help with this take it a bit further...

I will post back what I have come up with in case others are having the same issues regarding the sheet metal rule property...

Thanks Steven and Mike!

[Anonymous]

I wish I had the time to mess with iLogic rules and learn the proper formatting, but whenever I start, it never fails that we get swamped 🙂

[Anonymous]

Yea my position is pretty laid back, although it can get busy...gives me time to learn new things as well as troubleshoot issues...haha

I don't know much logic, but my tactic is,to use variants of what has been done...I don't typically do things that haven't been tried or done yet...so I just find bits and pieces and piece it together...

been working so far..but this forum helps tons!!

Thanks

[RobJV]

The easiest and slickest way I have found to do this is using a substitution rule on the material column in your partslist as well as using Brian Ekins addin.

Your partslist will automatically be populated and it works with all legacy parts as well.  Your material column will be populated with the sheetmetalstyle when it exists which is your gage and material. 

http://forums.autodesk.com/t5/Autodesk-Inventor/Parts-List-amp-BOM-amp-Stock-Number-amp-Sheet-Metal-...

Let me know if you have any questions.

[Anonymous]

I am not sure if this is a bug or has something to do with rules of programming, but I managed to get this to work!

In my Custom iProperty menu, I create a new property called Sheet Metal Rule and placed <Sheet Metal Rule> in the value input.

This was NOT working and it should have , BUT when I changed the name of the property to SheetMetalRule, (no spaces) it works!

Thanks to all who helped!

[Andrew1307]

The reason this was not working for you intially was because you were naming the custom property "Sheet Metal Rule" which is the same as what you you are trying to set it to. So when inventor looks for "Sheet Metal Rule" with =<Sheet Metal Rule> it was finding the custom name of "Sheet Metal Rule" and setting it to <Sheet Metal Rule>. Honestly i'm surprised this doesn't throw an error or cause issues as its an infinite loop. As soon as you removed the spaces this created a unique property name for =<Sheet Metal Rule> to be applied to allow Inventor to grab the actual "Sheet Metal Rule" property. 

Thanks for this thread. I am currently going through the same issues setting up our new templates and want material thickness to be displayed in friendly manners (3/16" SM. AL. or 10ga MS, ect.)