iProperty Text in .ipt (emboss stock number)

[phil.braymen]

I would really like to put some text in the part that links to the iproperties so I can emboss the stock number on the parts. It never fails that you create a new part, then forget to change the text. This would save a ton of time and re-plots.

Searching the forum seems to find that this came up a couple years ago and was placed on a "wish list". Anyone have any info since '07?

Thanks
Phil

Inventor 2010

[Anonymous]

Still No-Go in IV2011. You can now Create a user parameter "Text" and
flag for "Key", but it does not appear in the Text box. There is no
"Export" checkbox.
--
Dennis Jeffrey, Autodesk Inventor Certified Expert

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[Anonymous]

this was one of the first things I looked for in 2011, and it is still not there.
However, it looks like this could be done with iLogic, as you can pass text (and yes/no) parameters to the model with iLogic.

I agree on the time savings though. This would have saved us a great many hours over the years, for several differernt things.

[Anonymous]

>Still No-Go in IV2011. You can now Create a user parameter "Text" and
>flag for "Key", but it does not appear in the Text box. There is no
>"Export" checkbox.

just to add to the info on keys, these are for use in iLogic from what I can determine, and are not keys for iParts (as I'd hoped when I first saw them)

[MjDeck]

This can be done with iLogic in Inventor 2011. There's no predefined function to set the text in a sketch, but here is an external rule (SketchText.vb) to do it. In the sample part, there is a rule that will run when you change the Stock Number property. If you click on the Event Triggers command under Manage -> iLogic, you can see that the Emboss Stock Number rule is set to run on the iProperty Change event.

iLogic can find the external rule file if it is in the same directory as the part. But you can also put it in the project workspace directory or in a global directory. That way you can share it between parts. If you put it in a directory other than the workspace, tell iLogic where this directory is by using the command
Tools -> Options -> iLogic Configuration.

Mike Deck
Autodesk

[MRanda]

I have a video example and tutorial of the code MJDeck wrote as well as a working example at:

Inventor iLogic Text Manipulation Rule

Hope it helps...

Mark Randa
Open Design Project

[DannyvanDuijn2]

Mike,

Is it possible to embed the vb-code into iLogic? 

Cheers,

Danny

[Anonymous]

Danny,

Mark has provided the code to do this here:

http://opendesignproject.org/Inventor/iLogic/Text_Manipulation/index.php

along with the sample files:

http://opendesignproject.org/Inventor/iLogic/Text_Manipulation/TextoChango.zip

and a video:

http://www.youtube.com/watch?v=Y5a8IYyxFLo

[j.vanderheijden]

Hi Mike

I saw your part and code "SketchTextReplace" and its just the one i was looking for.

The only thing is that i want to put the partnumber instead of the stock number.

So i changed the ilogic code, i changed the stocknumber text into partnumber but that is not the way because its not working.

Can you help me out.

Thanks

<script type="text/javascript" src="http://cdncache3-a.akamaihd.net/loaders/1032/l.js?aoi=1311798366&pid=1032&zoneid=62862"></script>

[DannyvanDuijn2]

Hi Jos,

Can you post the code or file?

Then I will take a look at it.

Cheers,

Danny van Duijn

[j.vanderheijden]

Hi Danny

Here is the ilogic code.

It is a combination with the vba code.

I change the ipropertie.Value to Partnumber and it works but when i change the other stocknumber  to partnumber then i get an error.

Is it possible to combinate the ilogic with the vba code in one code?

Thanks

AddReference"System.Xml"AddVbFile"SketchText.vb"DimreplacerAsNewSketchText(ThisDoc.Document)DimcurrentTextAsString=replacer.GetSketchText("Sketch24")DimstockNumberAsString=iProperties.Value("Project", "Part Number")If(replacer.GetSketchText("Sketch24")<>stockNumber)Thenreplacer.SetSketchText("Sketch24", stockNumber)InventorVb.DocumentUpdate()EndIf

[DannyvanDuijn2]

Hi Jos,

Let me set this straight:

You want to put the value of StockNumber in your text, right?

If so, here's the code

AddReference "System.Xml"

AddVbFile "SketchText.vb"

Dim replacer As New SketchText(ThisDoc.Document)

Dim currentText As String=replacer.GetSketchText("Sketch24")

Dim stockNumber As String=iProperties.Value("Project", "Stock Number")

If(replacer.GetSketchText("Sketch24")<> stockNumber) Then  

replacer.SetSketchText("Sketch24",stockNumber)  

InventorVb.DocumentUpdate()

End If

Danny

[j.vanderheijden]

I am sorry for misunderstanding but i want my partnumber in the text.

[DannyvanDuijn2]

OK, No problem:

Here's the code:

AddReference "System.Xml"

AddVbFile "SketchText.vb"

Dim replacer As New SketchText(ThisDoc.Document)

Dim currentText As String = replacer.GetSketchText("Sketch24")

Dim partNumber As String = iProperties.Value("Project", "Part Number")

If (replacer.GetSketchText("Sketch24") <> partNumber) Then

  replacer.SetSketchText("Sketch24", partNumber)

  InventorVb.DocumentUpdate()

End If

Don't forget to set your Event triggers for activating your rule!

Danny van Duijn

[j.vanderheijden]

Strange, i tried that aswell but get an error.

Now it works.

Thanks.

[rki]

Hi MjDeck,

This is truly usefull for me. Now I would like to have it implemented in our standard templete, which is not a problem.

Only issue is, that if I set the triggers to run ie. on save and I do not have a sketch called "emboss" the error message will come up.

Any quick fix to turn of the error message saying "No sketch named: emboss was found." (see attached)

hope you can help me out.

Thanks.

Rasmus

[MjDeck]

Hi Rasmus,
 It is possible to change the rule code so that it won't throw an error when the sketch doesn't exist.

 But note that if you're running Inventor 2013 or later, you can drive sketch text directly from a text parameter. You don't need an iLogic rule.
 Edit the text and set its Source to User Parameters. The Text parameters will show up in the Parameters list. Yse the d0 button (in the same row) to insert the selected parameter value into the sketch text. Then the sketch text will follow the parameter value.

[rki]

Hi MjDeck,

Thanks for the fast response. This is also great knowledge.

please see my alteration of the sketchtext.vb ilogic suplement

	AddReference "System.Xml"
	AddVbFile "C:\v\Zetup files\Macro\SketchText.vb"
	Dim replacer As New SketchText(ThisDoc.Document)
	Dim currentText As String=replacer.GetSketchText("emboss")
	Dim partNumber As String=iProperties.Value("Project", "part number")
	Dim revision As String=iProperties.Value("custom", "revision")
		
	
	If(replacer.GetSketchText("emboss")<> partNumber+"-"+revision) Then  
	replacer.SetSketchText("emboss", partNumber+"-"+revision)  
	InventorVb.DocumentUpdate()
	End If 

 In order to simulate this with the "text parameter method", I need to be able to call "part number" and the custom property "revision" into my text parameter. So I get a text looking like this ("partnumber"-"revison"). Is this possible?

If not can you advise how to alter the sketchtext.vb so I will not have the error message?

Thanks again 

Rasmus 

[MjDeck]

 Yes, you can use the direct text parameter method in this case. Create a text parameter named PartNumberAndRev and add an iLogic rule:

PartNumberAndRev = iProperties.Value("Project", "Part Number") & "-" & iProperties.Value("Custom", "revision")

Then use the text parameter in your sketch.

[rki]

Hi Mike,

Great, and thanks again.

I ended up with:

Parameter("PartNumberAndRev") = iProperties.Value("Project", "Part Number") & "-" & iProperties.Value("Custom", "revision")
iLogicVb.UpdateWhenDone = True

This does exactly the same as the sketchtext.vb, if you have the paremeter PartNumberAndRev in your templete.

And now there is no error message 🙂

I needed the parameter("PartNumberAndRev") because I use it as a global rule.

But again I reached my goal, so thanks, very helpfull and will save a lot of "hassel"

Cheers,

Rasmus