topic Re: Inventor Assembly Half-Section View in Inventor Forum

Inventor Assembly Half-Section View

stuart_bassil — Thu, 19 Jan 2023 10:23:47 GMT

I am trying to create an half-section view of a complex assembly. When I first create the view I can either drag the pointer up and down or I can type in a specific dimension. My question is: Is there a way to edit that dimension once the view has been created?

Re: Inventor Assembly Half-Section View

CCarreiras — Thu, 19 Jan 2023 11:44:34 GMT

Hi!

I believe is not possible.

Re: Inventor Assembly Half-Section View

jtylerbc — Thu, 19 Jan 2023 20:28:36 GMT

No, that doesn't really seem to be a value that is stored by Inventor. You just re-create the section and enter the new value.

Re: Inventor Assembly Half-Section View

stuart_bassil — Fri, 20 Jan 2023 08:16:54 GMT

Thanks. I suspected as much but I thought I'd ask the question in case I was missing something.

Re: Inventor Assembly Half-Section View

mluterman — Fri, 20 Jan 2023 13:37:14 GMT

For complicated sections, I do a sketch, split it and then derive it (the section I want to look at) into a separate .ipt; this way you can control that dimension. Yes, it's a separate file, but it will update with the sketch and you're only limited by your imagination, not just some orthogonal cut lines.

Re: Inventor Assembly Half-Section View

Bert_Bimmel — Thu, 13 Apr 2023 13:36:48 GMT

You're right: The face you pick and the offset-value you type are completely volatile: What remains in memory is a dumb fixed plane defining the slice. In the DesignViewRepresentation that may be saved to the file there is no offset stored either, nor does it contain any referencekey to the picked face.

Your best shot would probably be to get the sectionplane-data from the API, and translate its root point by a multiple of its normal:

Sub MoveSectionViewPlane(Offset As Double) Dim SectViewPlane1 As Plane Dim SectViewPlane2 As Plane Dim SectionType As SectionViewTypeEnum Dim NewSectPlaneRootPt As Point Dim NewSectionPlane As Plane Dim SectPlaneNormal As Vector Call ThisApplication.ActiveDocument.ComponentDefinition.RepresentationsManager.ActiveDesignViewRepresentation.GetSectionViewInfo(SectionType, SectViewPlane1, SectViewPlane2) Set NewSectPlaneRootPt = SectViewPlane1.RootPoint.Copy Set SectPlaneNormal = SectViewPlane1.Normal.AsVector Call SectPlaneNormal.ScaleBy(Offset) Call NewSectPlaneRootPt.TranslateBy(SectPlaneNormal) Set NewSectionPlane = ThisApplication.TransientGeometry.CreatePlane(NewSectPlaneRootPt, SectViewPlane1.Normal.AsVector) Call ThisApplication.ActiveDocument.ComponentDefinition.RepresentationsManager.ActiveDesignViewRepresentation.SetSectionView(SectionType, NewSectionPlane, SectViewPlane2) End Sub

(This is for a half section view only, but it might inspire you to adapt it to some quarter section view if needed)

Re: Inventor Assembly Half-Section View

dusan.naus.trz — Tue, 05 Mar 2024 23:33:24 GMT

I found something. I tried to use it and it doesn't work. He writes about SendKeys there. Is it possible to use this in iLogic?

https://adndevblog.typepad.com/manufacturing/2012/06/run-half-section-view-command-in-assembly-through-api.html

Re: Inventor Assembly Half-Section View

CCarreiras — Wed, 06 Mar 2024 09:45:06 GMT

I believe it's possible.

If you can ask the Inventor to create a section in an existent plane, and you can also change the plane offset (previously), this could be a nice workaround to create a "dynamic" section view.

I would create a ilogic form to insert the plane offset and a button to run the section view command...

Re: Inventor Assembly Half-Section View

Bert_Bimmel — Wed, 06 Mar 2024 10:05:13 GMT

Apparently you haven't read (or understood) my previous post. Inventor "forgets" the plane you've picked as soon as you apply your section view.

Anyway, the proposed solution from my post above has become obsolete when Autodesk has implemented this by themselves somewhere between 2020 and 2024.

This is one of the rare cases where I must admit, that they have come up with a GOOD solution: Now you can not just move, but even TURN your section view plane.

So, unless you want to stay with an earlier Version of Inventor (which i can totally understand), your problem IS solved.

Re: Inventor Assembly Half-Section View

dusan.naus.trz — Wed, 06 Mar 2024 10:08:09 GMT

@Bert_Bimmel Now the question is how to connect iProperty OFFSET to SendKeys?

info

What is the thought or intention? Why do users want this functionality? Explanation: I'm trying iLogic with Measure. I am able to get the Measure into the iProperty, but I don't know how to get the SendKeys. I've tried it through setting planes and offsets and it's too complicated. If I could get into Senkeys it would solve a lot, because I would measure through iLogic and I would immediately have a half cut at the Measure location.

Re: Inventor Assembly Half-Section View

CCarreiras — Wed, 06 Mar 2024 10:43:18 GMT

@dusan.naus.trz , i suggest you open a new tread in a in inventor iLogic forum.
There will be there more capable people to help you on this, for sure.

BTW... My idea was about an offset for a work plane already existent, not directly in the section tool.
After placing the plane with a selected offset, the half section tool selects that plane to section the part.

Re: Inventor Assembly Half-Section View

Bert_Bimmel — Wed, 06 Mar 2024 11:18:01 GMT

I still don't get your desired workflow.

Do you want to send ctrl-c to capture something from your Measure-Dialog and use it somewhere later in your code, or what?

Anyway, SendKeys seems to be a member of VBA and is as easy to use as it appears useless to me: my suggestion won't work, 'cause either...

as soon as you start the macro via UI-Button the text that you have marked for capturing loses focus and nothing will be captured, or...

when you have assigned a keyboard-shortcut to your macro, it won't run as long as something is marked for beeing captured.

If you though still insist on having some similar functionality in iLogic, i guess you'll have to use some WinAPI-functions.

LMGTFY:

Already been here

https://forums.autodesk.com/t5/inventor-forum/sendkeys-or-keystrokes-using-ilogic/td-p/3346779

😉

Re: Inventor Assembly Half-Section View

dusan.naus.trz — Wed, 06 Mar 2024 11:53:15 GMT

Iam getting this error: for iLogic

Rule compilation errors in: Custom_Half_Section_View, in: Assembly1.iam Error on line 4: The SendKeys type is not declared and is likely to be inaccessible due to the protection level.

ThisApplication.CommandManager.ControlDefinitions.Item("AssemblyHalfSectionViewCmd").Execute2(True)

'Public Sub TestSendKeys()
SendKeys ("{20}")
'End Sub

Re: Inventor Assembly Half-Section View

Bert_Bimmel — Wed, 06 Mar 2024 11:59:42 GMT

What I've just said:

"The SendKeys type is not declared..."

In other Words "I (iLogic) have no clue what "SendKeys" is!"

-> Its availlable in VBA, not in iLogic. You'll probably have to use PostMessageA from user32.dll instead.