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Scotty87
Posts: 17
Registered: ‎02-16-2012
Message 1 of 19 (2,639 Views)

Component View Item Numbers – Methods and Suggestions

2639 Views, 18 Replies
06-14-2012 06:28 AM

Hi all,

After a bit of thought I’ve decided to do a write up on issues with item numbers in Inventor drawings. My reasons for this are that I want to know if there any ways to do what I want to do that I haven’t discovered, describe some current methods that some of you might find useful, and get support and/or criticism for a new feature that I am going to present.

 

As a draftsman with 4 years + experience with Inventor, I have come to know the program fairly well and regard it highly.

 

There is however one major flaw with the drawing environment: The inability (there are workarounds, which I will get to shortly) to attach an item number to component detail views that reference the BOM of their parent assembly.

This may seem trivial, but is a subject that keeps coming up, not just from Inventor users but also from other design office personnel, allocation staff and manufacturing workers.

 

I won’t rule out the possibility that this feature exists (if it does, please enlighten me!), but I would like to know why such an important feature has been omitted. Legal/copyright reasons? Marketing reasons? It’s not possible to program it that way? Not seen as important? In development?

 

Whatever the case, I will now discuss 3 workaround methods, followed by my own suggestion as to how I believe this feature could/should be included.

 

Method 1: iProperties Item Reference

Using this method, the item column and item bubbles reference an iProperty (such as Part Number or Stock Number) rather than the Item Number found in the BOM. A base view of an assembly is placed on a drawing, followed by base views of its parts. A parts list referencing the assembly is then created, and item balloons are attached to all parts on the assembly view and all component base views.

Advantages of this method include:

  • Ability to attach item balloons to each component base view.
  • Ability to include the item number in component view labels.

Disadvantages include:

  • Item numbers must be entered manually.
  • Item number is an iProperty; if a component is being used in multiple drawings, it retains its original item number. If the item number is changed to suit a new drawing’s BOM, the original drawing’s BOM will also update.
  • Does not allow for automatic renumbering in the parts list editor.

Method 2: Component View Representations

In the assembly, a new view representation is created for each component, in which visibility for every other component is switched off. A base view of the assembly is placed on a drawing with the relevant view representation selected for each part detail.

Advantages:

  • Allows ballooning of component views using BOM Item Number.
  • Quantity can be added to balloons and view labels.

Disadvantages:

  • Creation of view representations is time consuming.
  • A new view representation must be created for each new component.
  • Visibility of newly placed components must be manually deselected.
  • iProperties in view label reference parent assembly
  • Inability to detail flat pattern views.

Method 3: Weldment Detail

This method is similar to the view representation method, however the views are created automatically. It has the disadvantage that a weldment must be created for it to be of any use; as such it has no use for fastened assemblies that require component details.

 

These 3 methods all have their pros and cons, and really only appear to be workarounds for the problem at hand.

 

Now to my suggestion:

 

COMPONENT VIEWS

 

First, a standard base view of an assembly is placed on the drawing.

In the drawing environment, on the views panel of the drawing tab, there will be a button titled “Component Views”.

Pressing this button will bring up a prompt that says “select source view”.

The user then clicks on the base view on the assembly, and a dialogue box appears.

The box has a list of the assembly’s components, each next to a check box. The user then checks the required components, or checks “select all”.

The user then places each component view 1 by 1, selecting orientation as they go.

Item balloons can now be added to the component views; the number reflects the item number in the parts list of the parent view.

BOM data can also be added to the view label via “BOM Properties” in the drop down menu, and “Component Properties” references the iProperties of the component; Model Properties still allows the parent assembly to be referenced.

The component view can be turned into a standard base view by right clicking it and selecting “convert to base view”. I would also endorse the possibility of converting base views to component views.

 

I’m no expert on the programming side of things, but I don’t see why this isn’t possible; all the information is there, it seems like it’s a matter of getting it all in the one place.

 

Please let me know what you think about the component views idea. Preferably quote one of the following points

  • Great idea! Autodesk, take note.
  • Sounds good, but needs more thought.
  • Not that important, but it can’t hurt to have it.
  • Some good points, but lots of flaws; I am happy without it.
  • No good, completely unnecessary / totally flawed.

 

Thanks for reading, constructive criticism is greatly appreciated.

*Expert Elite*
PaulMunford
Posts: 891
Registered: ‎11-13-2006
Message 2 of 19 (2,630 Views)

Re: Component View Item Numbers – Methods and Suggestions

06-14-2012 08:00 AM in reply to: Scotty87

I think that the answer may be semantic - but this is how I am coming to understand it.

 

The assembly Item No. is only meant to be used to call out the part numbers on the current drawing (or set of drawings). i.e. the drawings for one assemblyThis is how engineering drawings have always worked.

 

If you are creating a 'piece part' drawing, then you shouldn't need to refer to an assembly item No., because only one part is shown on the drawing.

 

To reference the part to the assembly drawing you would use a unique Part Number.

 

So the drill down would look like this.

 

Assembly drawing > Parts list > Item No. > Part Number

 

In theory, you don't need to go the other way, beacuse a part could be used in many different assemblies. Each assembly however, is unique.

 

I'm not saying that there is no need for the feature as you describe, I'm only saying that Inventor was designed to work using a traditional engineering process.

The CAD Setter Out Blog @CadSetterOut

Inventor Surfacing | AutoCAD | CAD Standards
 
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jtylerbc
Posts: 864
Registered: ‎09-01-2010
Message 3 of 19 (2,627 Views)

Re: Component View Item Numbers – Methods and Suggestions

06-14-2012 08:20 AM in reply to: PaulMunford

Paul's explanation is correct.  Inventor's way of handling the item numbers is optimized for a manufacturing environment with unique parts identified by part numbers.

 

In that sort of an environment, each of these parts gets its own individual drawing, rather than being a "detail view" related to an assembly drawing.  The assembly item number is not shown on this drawing, because it isn't needed and in many (if not most) cases there will actually be more than one.

 

What we're really talking about here is a difference in drawing styles between manufacturing and fabrication.  Inventor's setup is optimized for the manufacturing conventions, and requires a bit of improvisation for fabrication.  Having come from a manufacturing-based company to a fabrication based one a couple of years ago, these differences in thinking are something I deal with regularly.

 

Since we had some inconsistency in our drawing formats anyway, I picked one of the used conventions that was more Inventor-friendly and made it the standard.  We don't use the Item Number at all on our fabrication drawings.  Instead, we use "Mark Number", which is really just a renamed "Part Number" column in the parts list.  I then put the Part Number iProperty in the view labels for the details.

 

Isn't really a true solution for what you're asking for, but it sidesteps the issue and works for us.

John Tyler
Inventor 2013
Windows 7 64 Bit
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Curtis_Waguespack
Posts: 2,780
Registered: ‎03-08-2006
Message 4 of 19 (2,600 Views)

Re: Component View Item Numbers – Methods and Suggestions

06-14-2012 09:51 AM in reply to: Scotty87

Hi Scotty87,

 

A few quick questions:

 

  • What version of Inventor are you using?
  • Are you open to using ilogic to help with this?
  • Can you provide a simple example data set and/or screen shots that will illustrate your goal(s)?

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



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PaulMunford
Posts: 891
Registered: ‎11-13-2006
Message 5 of 19 (2,601 Views)

Re: Component View Item Numbers – Methods and Suggestions

06-14-2012 12:29 PM in reply to: jtylerbc

Thanks for that jtylerbc, I'm glad I wasn't baring up the wrong tree!

 

That's and interesting point that you make about manufacturing Vs Fabrication. I also work infabrication and I have trying to get the Assembly Item No. to do somrthing I am begining to think it wasn't inteded for. 

 

It's good to get some validation :smileyhappy:

 

Paul

The CAD Setter Out Blog @CadSetterOut

Inventor Surfacing | AutoCAD | CAD Standards
 
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jtylerbc
Posts: 864
Registered: ‎09-01-2010
Message 6 of 19 (2,596 Views)

Re: Component View Item Numbers – Methods and Suggestions

06-14-2012 12:58 PM in reply to: PaulMunford

Taking my explanation just a bit further:

 

We annotate these types of drawings with a balloon style that uses the Part Number property rather than the Item Number.  So, there is never actually an "Item Number" anywhere on the drawing.

 

I actually have parts lists and balloon styles set up for both types of formats.  We do steel fabrication (frames) as well as final assembly of other components (hydraulics, etc) for our equipment.  The method I've been describing works well for the steel fabrication drawings, and looks like one of the more common formats of our previous AutoCAD work.

 

However, it is very messy for purchased parts, which might have long model codes as the part number.  The normal way of using Item Numbers and balloons in Inventor works much better for these drawings.  I use two different Standards to set the default styles appropriately for the particular drawing.

 

It's a very simple fix if you can get away with using the Part Number field instead of the Item Number.  Even if you don't want to put it in the view label, and instead want to use a balloon on the detail views, the Part Number property is still the same whether you're looking at the part in an assembly or by itself.

John Tyler
Inventor 2013
Windows 7 64 Bit
Contributor
Scotty87
Posts: 17
Registered: ‎02-16-2012
Message 7 of 19 (2,571 Views)

Re: Component View Item Numbers – Methods and Suggestions

06-14-2012 11:01 PM in reply to: jtylerbc

Thanks for the replies!

 

@ Paul Munford and jtylerbc:

 

FYI, I'm from Australia (guessing you guys are from the US?), so my drafting techniques are going to be based on Aus standards; for the most part I'm not sure how other countries operate.

In any case, I've done drafting work for 4 companies in 4 different industries (marine oil, recycling, water purification and currently coal mining), and every one of them will create a drawing that contains an assembly or weldment and on the following sheets (sometimes, as in my attachments, the same sheet) or a new drawing file, detail views of the constituent parts. Some parts do get a drawing all to themselves though, as do subassemblies.

As for fabrication drawing vs. manufacturing drawings, even if Inventor is optimised for one over the other, there is no reason why it shouldn't be able to better accommodate the other. Both have their merits and are important for manufacturing.

The concept of using unique iProperties as mark numbers would definitely be good in some applications, but it's not really what I'm getting at. The company I'm with now uses part numbers that are usually the same as the file number to identify parts (see attachments), however the long part numbers are difficult to read and usually don't follow any logical order. Also, I mentioned in my original post using iProperties to identify parts; the difference being that your suggestion implies unique mark numbers whereas I was implying a substitute for item numbers.

Also note that the component views feature that I suggested shouldn't in any way affect the way you create drawings/views etc; it would still allow you to create a drawing exactly as you do today, but with the added option of creating linked views that can be annotated with data from both the part itself and its parent's BOM.

 

@ Curtis_Waguespack:

 

I'm currently using Inventor 2012 Professional (full version at work, student version at home).

Yeah, I'm open to using iLogic. I've managed to get component quantities using it, but no such luck with item numbers.

See attached files.

Fig1 shows what I want to achieve, using both part iProperties and BOM properties (Item, Qty).

Fig2 shows a drawing similar to what I would create where I work now.

BTW, I'm currently reading Mastering Inventor 2012 and it's great! Only up to chapter 4 and I'm already picking up on lots of little things that I had previously overlooked. 

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jtylerbc
Posts: 864
Registered: ‎09-01-2010
Message 8 of 19 (2,547 Views)

Re: Component View Item Numbers – Methods and Suggestions

06-15-2012 05:53 AM in reply to: Scotty87

I wasn't saying it shouldn't do both, was just explaining the reasoning behind what it currently does.  It would be nice to have the option of both for those who need it.  With the amount of structural steel stuff in the Content Center, it would seem to make sense to make the drawing annotation a bit more fabrication-friendly.

 

I think iLogic is probably going to be your best bet.  Another possibility, which I've seen used on some of our older Inventor drawings, is to use View Representations.  Instead of placing views of the individual parts, you would create View Reps in the assembly that turn off all but one part, then place a view of that.  Since your view is still the assembly, the item numbers still work correctly.  I think this is the closest currently-existing option to your "component view" suggestion.

 

However, if you have any information you want to pull from the part into the view label (part number, etc), this method will mess that up (because the view technically isn't of the part).

John Tyler
Inventor 2013
Windows 7 64 Bit
Contributor
Scotty87
Posts: 17
Registered: ‎02-16-2012
Message 9 of 19 (2,537 Views)

Re: Component View Item Numbers – Methods and Suggestions

06-15-2012 08:32 AM in reply to: jtylerbc

Re: first paragraph, I (almost) agree completely. Only rather than thinking it would be a nice addition, I'm thinking "why the f*** haven't they done this already?!"

 

Case in point: One of the pre production/allocation staff members where I currently work has gone to the extent of adding item balloons to each part base view in red pen on printed drawings so he has an easy way of linking the views to the parts list. Also as I've already mentioned, this isn't an isolated need; 4 out of 4 places I've worked at include multiple part details on a single drawing.

 

Re: second paragraph, I have played around with iLogic and have managed to get quantities out of it but still can't do anything with item numbers. So far I only have limited experience with iLogic though, and wouldn't be surprised if it could solve my issues. As for view representations, I mentioned this method in my original post, including the reasons why I think it is insufficient. I do agree however that it probably is the closest existing method to what I want to achieve.

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Curtis_Waguespack
Posts: 2,780
Registered: ‎03-08-2006
Message 10 of 19 (2,522 Views)

iLogic: Create a View Representation for Each Part In theAssembly

06-15-2012 10:35 AM in reply to: Scotty87

Hi Scotty87,

 

Thanks for the screen shots, that helps a great deal.

 

Let's take this one step at a time. To start off here is an iLogic rule that will create a view rep that islolates each part in the assembly. If more than one instance of the part is present it isolates just the first one. If a Default view rep is present the rule honors the visibility settings you might have adjusted previously. If no Default view rep is found then it creates one and sets all parts visible.

 

Likewise if a view rep that has the same name as one of the parts is present then the rule honors it and makes no adjustments, but will create a view rep for each part name that isn't present as a view rep. Once the view reps are created they are locked

 

Give it a test and see what you think. I currently have the display updating as the view reps are created so you get some visual feedback, but let me know if that runs too slowly.

 

I'll look at the drawing views next (as time permits).

 

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


 

 

 

'define current document
Dim openDoc As Document
openDoc = ThisDoc.Document

' set a reference to the assembly component definintion.
' this assumes an assembly document is open.
Dim oAsmCompDef As AssemblyComponentDefinition
oAsmCompDef = ThisApplication.ActiveDocument.ComponentDefinition

'look at all of the components in the assembly
Dim oCompDef As Inventor.ComponentDefinition = openDoc.ComponentDefinition

'define the first level components collection
Dim oCompOcc As Inventor.ComponentOccurrence 

'define view rep 
Dim oViewRep As DesignViewRepresentation

'define an arraylist to hold the list of  view rep names
Dim NameList As New ArrayList()

'Look at the view reps in the assembly
For Each oViewRep in oAsmCompDef.RepresentationsManager.DesignViewRepresentations
'set the list of names to the array list
NameList.add(oViewRep.Name)
Next

'check for a Default view rep and create it if not found
If Not NameList.Contains("Default") Then
	'create Default view rep 
	oViewRep = oAsmCompDef.RepresentationsManager.DesignViewRepresentations.Add("Default") 
	oViewRep.ShowAll
	oViewRep.Activate
End If

'zoom all
ThisApplication.CommandManager.ControlDefinitions.Item("AppIsometricViewCmd").Execute

'look at all of the unique parts in the assembly
For Each docFile In openDoc.AllReferencedDocuments
	If docFile.DocumentType = 12290 Then '12290 is the part document enumurator
	'locate the last backslash position in the full file name
	Dim FNamePos As Long
	FNamePos = InStrRev(docFile.FullFileName, "\", -1) 
	'remove path from part file name 	
	Dim docFName As String
	docFName = Right(docFile.FullFileName, Len(docFile.FullFileName) - FNamePos)         
	'remove extension from part file name 
	ShortName = Left(docFName,  Len(docFName) - 4)   
		'check to see if the arraylist contains the desired view rep
		If Not NameList.Contains(ShortName) Then
		'create new View Rep 
		oViewRep = oAsmCompDef.RepresentationsManager.DesignViewRepresentations.Add(ShortName)
		oViewRep.Activate
		oViewRep.Locked = False	
		Else if NameList.Contains(ShortName) Then
		'reference existing View Rep 
		oViewRep = oAsmCompDef.RepresentationsManager.DesignViewRepresentations.Item(ShortName) 
		oViewRep.Activate
		oViewRep.Locked = False
		End If
		'look at all of the occurences
		For each oCompOcc in oCompDef.Occurrences
		'locate the colon position in the occurence name
		oCompOccPos = InStrRev(oCompOcc.Name, ":") 
		'set occurence name to everything left of the colon
		oOccName = Left(oCompOcc.Name, oCompOccPos -1) 
			'set visible if name matches first occurence
	      		If oCompOcc.Name = ShortName & ":1"  Then
			oCompOcc.Visible = True
			ThisApplication.ActiveView.Update()
			Else
			oCompOcc.Visible = False
			ThisApplication.ActiveView.Update()
			End If
		Next
	End If
	'lock view rep
	oViewRep.Locked = True	
Next

'set Default View Rep active
oAsmCompDef.RepresentationsManager.DesignViewRepresentations.Item("Default").activate

 



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