Inventor 2014, Detail Multiple Parts on a Single sheet

[Adam.Zarate]

In Inventor 2014, Can you detail multiple parts on a single drawing sheet? I have 2 parts made from sheet metal and using text to annotate the parts. I found that for the first part I place, I can use the following format withing the editor window "P/N : <PART NUMBER>[return]<DESCRIPTION>[return]Material : <THICKNESS> x <FLAT PATTERN EXTENTS WIDTH> x <FLAT PATTERN EXTENTHS LENGTH>, <MATERIAL>" where I can select from Type, Property, Component, Source and Parameter. This works for the first part placed, but not the second part placed. These drawing are for material cutting and bending prior to welding together and differ in shape.

Is there any way to do this without creating a sheet for each part.

Also, Is there a way to extract the BOM from a single sheet with these parts placed.

Please not these parts are not part os an assembly as of yet.

[mdavis22569]

Are you filling this in on the Part.idw level and not in the IPT  ..

if you're doing it in the Idw then I believe you can only get the one parts detail.

However if you do it in the ipt then you can do them separately. You can make separate BOM's and export them separately too.

[LT.Rusty]

Unfortunately, there is no way to pull the iProperties from anything other than the first model placed on a sheet.  If you have sketch symbols - or other text objects - which are calling iProperties from a model, you're only going to get the data from the first item you place.

If you need to call the iProperties for your annotation - because yeah, if you've got all this automation built in with the iProperties, it's annoying to have to re-type all the information - then you'll need to put your parts on separate sheets.

As far as the BOM goes, you CAN put more than one on a sheet, and when you place them, you can pick which view they'll be associated with.  You could, conceivably, add columns to it to reflect the additional iProperties you want to show, and then display your stock width or whatever in the form of a table.  This could go on a single sheet.  You'd have to play with the parts list table formatting.

[Adam.Zarate]

That's what I thought, but as you know there is always a way. So i'm
thinking is there a way to show the control codes for example
EXTENTS LENGTH>? I remember back in the Autocad days you had to know them.
My thought is if they are available in the Text Editor, there must be a way
to point to the correct IPT data.

As for puting the data in the Iproperties, I'm having the same issue trying
to reference the aforementioned value.

Any clues?

Thank You
Adam C. Zarate

[LT.Rusty]

---

@Adam.Zarate wrote:
That's what I thought, but as you know there is always a way. So i'm
thinking is there a way to show the control codes for example
EXTENTS LENGTH>? I remember back in the Autocad days you had to know them.
My thought is if they are available in the Text Editor, there must be a way
to point to the correct IPT data.

As for puting the data in the Iproperties, I'm having the same issue trying
to reference the aforementioned value.

Any clues?

Thank You
Adam C. Zarate

---

Okay, so this is a screenshot of the text edit window that you get for pretty much everything in the drawing environment.  I've circled three things in it.

Use the pulldown circled in black to pick the type of property you want to access.  These properties are drawn from one or another of a variety of other sources.  The pulldown marked Property, circled in red, is where you pick which individual one you want.  The button circled in green will insert the value in the text box.

The only way to pick which model or assembly you pull these details from is to make sure that you put the one you want to use on the sheet first.  Hopefully this will change in a future release ... there's times when I have planned poorly and would love to be able to change where these data points are captured from, but the only way to do that is to start a new page, put something different on the sheet, then copy the rest of my views over there.

The sheet metal extents that you were looking for are located - perhaps obviously - under SHEET METAL PROPERTIES on the TYPE menu, which is the one circled in black.

[rhasell]

Hi

I had to read your post carefully, and the catch is the "Use Text" The text will only associate it's self to the first part, as mentioned earlier.

There are two ways to get around this one:

1: Use the View Annotation to place the details.

This will be unique for each part.

2: Use a Leader.

 Change the style of the leader, to show or hide the line and arrow etc.

The iProperties will update when you attach it to a part.

The Leader can be copied and pasted from part to part, and will update accordingly.

[Adam.Zarate · Accepted solution]

Thank you all so much for getting back to me.
I was able to Find a work around that works great, thinking out of the box, I decided to populate the "Component" drop down of the Text Editor.

See the attached PDF and share

I surley hopes this helps other users

[jletcher]

LT. Rusty:

Unfortunately, there is no way to pull the iProperties from anything other than the first model placed on a sheet.  If you have sketch symbols - or other text objects - which are calling iProperties from a model, you're only going to get the data from the first item you place.

That is not correct LT you can get them from both if it is a symbol.. Just use the leader with Visible off (uncheck) and you can get the information from each part on a sheet..

[LT.Rusty]

---

@Anonymous wrote:

That is not correct LT you can get them from both if it is a symbol.. Just use the leader with Visible off (uncheck) and you can get the information from each part on a sheet..

---

Yep, I learned something new today.

[Curtis_Waguespack · Accepted solution]

Hi Adam.Zarate,

Here is an iLogic rule that will  look at each each view, on each sheet, of your drawing, and then it will add all of this information for you in the drawing view label, just as you show it in your PDF.

And here's a link to show you how to create a basic iLogic rule in your drawing:

http://inventortrenches.blogspot.com/2012/01/creating-basic-ilogic-rule-with-event.html

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

(see the attached file for the rule in a text file, just in case this code box messes with the formatting when copying and pasting.)

Dim oDoc As DrawingDocument:  oDoc = ThisDoc.Document
oModel = ThisDoc.ModelDocument

Dim oSheets As Sheets
Dim oSheet As Sheet
Dim oViews As DrawingViews
Dim oView As DrawingView

oSheets = oDoc.Sheets

'look at each sheet
For Each oSheet In oSheets
oViews = oSheet.DrawingViews
	'look at each view on the sheet
	For Each oView In oViews
	'Turn on the view Label
	oView.ShowLabel = true
	'get the model reference
	oModelName = _
	oView.ReferencedDocumentDescriptor.ReferencedDocument.DisplayName
	'get some standard iProperties from the model
	oPartNumber = iProperties.Value(oModelName, "Project", "Part Number")
	oDescription = iProperties.Value(oModelName, "Project", "Description")
	oMaterial = iProperties.Material(oModelName)
	
		'get custom iProps
		Try
		'get the property ID for these custom iProperties from the model referenced by the view
		o_iPropID_1 = oModel.PropertySets.Item("User Defined Properties").Item("Length").PropId
		o_iPropID_2 = oModel.PropertySets.Item("User Defined Properties").Item("Width").PropId
		o_iPropID_3 = oModel.PropertySets.Item("User Defined Properties").Item("Thickness").PropId
		Catch
		'here you could add a message that one or more of the custom iProperties were not found
		End Try
		
		'set iProp format to be able to use it in the View Label
		Try
		'_____ format the custom iProperty string and add the property ID
		oString1 = "<Property Document='model' PropertySet='User Defined Properties' " _
		&  "Property='Length' FormatID='{D5CDD505-2E9C-101B-9397-08002B2CF9AE}' PropertyID='" _
		& o_iPropID_1  & "'>Length</Property>"
		'_____ format the custom iproperty string and add the property ID
		oString2 = "<Property Document='model' PropertySet='User Defined Properties' " _
		&  "Property='Width' FormatID='{D5CDD505-2E9C-101B-9397-08002B2CF9AE}' PropertyID='" _
		& o_iPropID_2  & "'>Width</Property>"
		'_____ format the custom iproperty string and add the property ID
		oString3 = "<Property Document='model' PropertySet='User Defined Properties' " _
		&  "Property='Thickness' FormatID='{D5CDD505-2E9C-101B-9397-08002B2CF9AE}' PropertyID='" _
		& o_iPropID_3  & "'>Thickness</Property>"

		'add the custom iproperties to the view label
		oView.Label.FormattedText = "P/N : " & oPartNumber &  "<Br/>"  & _
		oDescription &  "<Br/>"  & _
		"Material : Sheet, " & oString3 & " Thk x " &   oString2 & " W x " &  oString1 &" L, " & oMaterial
		Catch
		'do nothing if error
		End Try
	Next
Next

[Adam.Zarate]

Thanks, I will check it out, but for now at least i'm out of hot water. I knew there was a better way to skin the cat