topic iLogic form in Inventor Programming Forum

iLogic form

JorisSteurs1246 — Fri, 14 Mar 2014 10:03:50 GMT

Does anyone knows if it is possible to add the selectionbox for the sheetmetal rule on an ilogic Form ?

Or if not possible, maybe some kinda workaround?

thanks

Joris

Re: iLogic form

GosponZ — Fri, 14 Mar 2014 17:19:47 GMT

Maybe tabs, i do have my rules dwg ipt and iam rules on different tabs. Working great. Just my 2 cents

Re: iLogic form

rjay75 — Fri, 14 Mar 2014 18:00:23 GMT

If the file is a Sheet Metal file this will fill a Text parameter with the sheetmetal styles. That parameter can then be added to a an iLogic form.

Dim smStyleList As New ArrayList

For Each smStyle As SheetMetalStyle In ThisDoc.Document.ComponentDefinition.SheetMetalStyles
	smStyleList.Add(smStyle.Name)
Next smStyle

MultiValue.List("paramName") = smStyleList

Re: iLogic form

JorisSteurs1246 — Fri, 14 Mar 2014 21:12:07 GMT

Thanks Rjay for this snippet, it works, and I have a slectable list on my form. Unfortunatly it goes only one way, the part doesn't change when selecting a new SheetStyle. That was actualy my aim. Maybe should have put my question a bit more precise :-).

Re: iLogic form

rjay75 — Fri, 14 Mar 2014 21:56:41 GMT

To go the other way create another rule with this

SheetMetal.SetActiveStyle(paramName)

When the parameter is update it should set the style.

Re: iLogic form

JorisSteurs1246 — Sat, 15 Mar 2014 14:13:00 GMT

Sorry to say but that last line didn't do the update.
This is what the total iLogic looks like right now.

Dim smStyleList As New ArrayList
For Each smStyle As SheetMetalStyle In
ThisDoc.Document.ComponentDefinition.SheetMetalStyles
smStyleList.Add(smStyle.Name)Next smStyle
MultiValue.List("SheetMetalType") = smStyleList
SheetMetal.SetActiveStyle(SheetMetalType)

Re: iLogic form

rjay75 — Sat, 15 Mar 2014 19:24:20 GMT

The last line has to be in a separate rule.

Re: iLogic form

JorisSteurs1246 — Sat, 15 Mar 2014 20:54:00 GMT

Tried this also, even added a document update rule, but the model keep his
thickness stubborn as it is.

Re: iLogic form

rjay75 — Sun, 16 Mar 2014 02:54:52 GMT

Hmm. I have gotten to work with two rules. The first rule looks like this.

Dim smStyleList As New ArrayList

For Each smStyle As SheetMetalStyle In ThisDoc.Document.ComponentDefinition.SheetMetalStyles
    smStyleList.Add(smStyle.Name)
Next smStyle

MultiValue.List("SheetMetalType") = smStyleList

The second rule looks like this.

SheetMetal.SetActiveStyle(SheetMetalType)

Each of these are regular rules.

I tested this on Inventor 2014. What version of Inventor are you running?

One thing to note is in the document I tested this it initially appeared not to work but it was because in the sheet metal defaults I didn't have Use Thickness From Rule checked,

Re: iLogic form

JorisSteurs1246 — Sun, 16 Mar 2014 09:22:00 GMT

Yes AI 2014 latest service pack.

Aaaand I got it working now. The problem was that I used external rules,
just a habit of mine to avoid making new templates all the time.
Strange though.... If I made it a normal rule it works fine , I'm going to
save both rules in the file and try if it still works when I trigger the
second rule on parameter change.

Anyhow already big thanks 🙂

Re: iLogic form

Anonymous — Mon, 20 Oct 2014 10:58:20 GMT

Hi all

I want to know if any of you had the experience of an smart form, for example consider a form with woth some parametes, as you can see in the attached picture, my first field, is a drop down menue showing the location of a nozzle, which might be located on top, shell or bottom of a tank, I want to be able to gray out some fields when I choose for example top situation, so, the grayed fields are not accessible and the user cannot write anything in those fields.

Thanks