Item Number on Drawing Views (multiple Parts Lists)

                If you remember, a while back I have created an ilogic code to add item number on drawing views (original post). Some companies like to detail parts along with assembles on same drawing or even on same sheet.

                I was doing a drawing for a frame and because there were mostly standard shapes that this frame was build out of I decided to document the rest of the components on same sheet. This was not an issue for my code but on frame generator drawings I don’t use a Parts list but rather a Material List.

                The difference is that it doesn’t have an “ITEM” column and so the code would fail to work. You can manually add a Parts List on the drawing outside the sheet but the code will still not work because it looks at the first PartsList on the sheet and in this case it was my Material List.

                Don’t get confused, Parts List, Material Lists, Cut-To-Length lists are all the same, just customized to show different info.

Parts List style

                Material Lists contains, total length, stock number, Description, Material and individual items are merged to show total quantity rather than number of each item.

Cumulated lengths 

                This is setup to work with Tube and Pipe members as well. Remember that Frame Generator use G_L as length and Pipes use PL for length and if you check the column settings for Quantity you will see that if the member is pipe (PL parameter exists) then it will use it as quantity.

Works with TP pipes.

                Now that we got that out of the way and familiarized ourself with the different type of Parts Lists let’s discuss the change in code.

                The original code was looking at the first parts list

        'oPartsList = oDrawDoc.ActiveSheet.PartsLists.Item(1)

                and we need it to search for a specific one “Parts List” so the code became

        For i=1 To oPartsLists.Count

               If oPartsLists.Item(i).Title = "PARTS LIST" Then

                       oPartsList = oPartsLists.Item(i)

                       Exit For

               Else

                'do nothing

               End If

        Next

                Here is the full code again version 1.3 (download link here)

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' Set a reference to the drawing document.

' This assumes a drawing document is active.

Dim oDrawDoc As DrawingDocument

oDrawDoc = ThisApplication.ActiveDocument

Dim oSheets As Sheets

oSheets = oDrawDoc.Sheets

Dim oSheet As Sheet'Inventor.Sheet

Dim oViews As DrawingViews

Dim oView As DrawingView

Dim oPartsLists As PartsLists

Dim oPartsList As PartsList

For Each oSheet In oSheets

    'declare the PartsLists 

    oPartsLists = oSheet.PartsLists

            'try and get the parts list form the table of this sheet

            Try

                'this doesn't work when you have a material list like on frame drawings

                'oPartsList = oDrawDoc.ActiveSheet.PartsLists.Item(1)

                'place a parts list on the drawing and search for it 

                'rather than using an id number

                For i=1 To oPartsLists.Count

                    If oPartsLists.Item(i).Title = "PARTS LIST" Then

                        'MessageBox.Show("found table", "ilogic")

                        oPartsList = oPartsLists.Item(i)

                        Exit For

                    Else

                        'do nothing

                    End If

                Next

            Catch 'on error try and search all sheets for first found parts list            

                'iterate trough each sheet

                Dim j As Long

                For j = 1 To oDrawDoc.Sheets.Count

                    If oDrawDoc.Sheets.Item(j).PartsLists.Count > 0 Then Exit For

                Next

                'this doesn't work when you have other parts lists like a 

                '"material list" like on frame drawing

                'oPartList = oDrawDoc.Sheets.Item(i).PartsLists.Item(1)

                'place a parts list on the drawing and search for it 

                'rather than using an id number to locate the first

                For i=1 To oPartsLists.Count

                    If oPartsLists.Item(i).Title = "PARTS LIST" Then

                        'MessageBox.Show("found table", "ilogic")

                        oPartsList = oPartsLists.Item(i)

                        Exit For

                    Else

                        'do nothing

                    End If

                Next

                'MessageBox.Show("parts list found on: " & j, "Title")

            End Try

    oViews = oSheet.DrawingViews            

    For Each oView In oViews

        'Get the full filename Of the view model

        Dim oModelFileName As String

        oModelFileName = oView.ReferencedDocumentDescriptor.ReferencedDocument.FullFileName

        'MessageBox.Show("view model name" & oModelFileName, "Title")

            ' Iterate through the contents of the parts list.

            Dim j As Long

            For j = 1 To oPartsList.PartsListRows.Count

                ' Get the current row.

                Dim oRow As PartsListRow

                oRow = oPartsList.PartsListRows.Item(j)

                'get filename of model in row

                Dim oRowFileName As String

                Try ' try and get the full file name of the PL item

                    oRowFileName = oRow.ReferencedFiles.Item(1).FullFileName

                Catch 'on error go to next item

'                    Dim oCellValue As String

'                    oCellValue = oRow.Item("Item").Value

'                    MessageBox.Show("Error Processing item: " & oCellValue, "Title")

                    Continue For

                End Try

                'compare the filenames

                'Performs a text comparison, based on a case-insensitive text sort order

                'If strings equal returns 0

                If StrComp(oModelFileName, oRowFileName, CompareMethod.Text)=0 Then 

                    'Get the value of Item from the Parts List

                    'Row name needs to be case sensitive or use 1 for first 2 for second etc.

                    oCell  = oPartsList.PartsListRows.Item(j).Item("Item") 

'Row name needs to be case sensitive or use 1 for first 2 for second etc.

                    'get the value of text in cell

                    Dim oItemValue As String

                    oItemValue = oCell.Value

                    'Show the view label

                    oView.ShowLabel = True

                    'format the text first line

                    oStringItem = "<StyleOverride Underline='True' FontSize='0.35'> ITEM " & oItemValue & " </StyleOverride>"

                    'format the text second line

                    oStringScale = "<Br/><StyleOverride FontSize='0.3'>(Scale <DrawingViewScale/>)</StyleOverride>"

                    'add to the view label

                    oView.Label.FormattedText =  oStringItem & oStringScale

                End If  

            Next

      Next

Next

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EDIT: 11/08/16
if you would rather be prompted to select views rather than processing all of them , here is the code.

------------------------------------------------------------------------------------------------------------

' Set a reference to the drawing document.
' This assumes a drawing document is active.
Dim oDrawDoc As DrawingDocument
oDrawDoc = ThisApplication.ActiveDocument
 
Dim oSheets As Sheets
oSheets = oDrawDoc.Sheets
Dim oSheet As Sheet'Inventor.Sheet
Dim oViews As DrawingViews
Dim oView As DrawingView
Dim oPartsLists As PartsLists
Dim oPartsList As PartsList
 
For Each oSheet In oSheets
    'declare the PartsLists 
    oPartsLists = oSheet.PartsLists
 
            'try and get the parts list form the table of this sheet
            Try
                'this doesn't work when you have a material list like on frame drawings
                'oPartsList = oDrawDoc.ActiveSheet.PartsLists.Item(1)
                'place a parts list on the drawing and search for it 
                'rather than using an id number
                
                For i=1 To oPartsLists.Count
                    If oPartsLists.Item(i).Title = "PARTS LIST" Then
                        'MessageBox.Show("found table", "ilogic")
                        oPartsList = oPartsLists.Item(i)
                        Exit For
                    Else
                        'do nothing
                    End If
                Next
                
            Catch 'on error try and search all sheets for first found parts list            
                'iterate trough each sheet
                Dim j As Long
                For j = 1 To oDrawDoc.Sheets.Count
                    If oDrawDoc.Sheets.Item(j).PartsLists.Count > 0 Then Exit For
                Next
                            
                'this doesn't work when you have other parts lists like a 
                '"material list" like on frame drawing
                'oPartList = oDrawDoc.Sheets.Item(i).PartsLists.Item(1)
                'place a parts list on the drawing and search for it 
                'rather than using an id number to locate the first
            
                For i=1 To oPartsLists.Count
                    If oPartsLists.Item(i).Title = "PARTS LIST" Then
                        'MessageBox.Show("found table", "ilogic")
                        oPartsList = oPartsLists.Item(i)
                        Exit For
                    Else
                        'do nothing
                    End If
                Next
                'MessageBox.Show("parts list found on: " & j, "Title")
            End Try
            
    oViews = oSheet.DrawingViews            

        'get view from user
        While True
            oView = ThisApplication.CommandManager.Pick( _
            SelectionFilterEnum.kDrawingViewFilter, "Select a View") 
        
            'Get the full filename Of the view model
            Dim oModelFileName As String
            oModelFileName = oView.ReferencedDocumentDescriptor.ReferencedDocument.FullFileName
            'MessageBox.Show("view model name" & oModelFileName, "Title")
                
            ' Iterate through the contents of the parts list.
            Dim j As Long
            For j = 1 To oPartsList.PartsListRows.Count
                ' Get the current row.
                Dim oRow As PartsListRow
                oRow = oPartsList.PartsListRows.Item(j)
                'get filename of model in row
                Dim oRowFileName As String
                Try ' try and get the full file name of the PL item
                    oRowFileName = oRow.ReferencedFiles.Item(1).FullFileName
                Catch 'on error go to next item
'                    Dim oCellValue As String
'                    oCellValue = oRow.Item("Item").Value
'                    MessageBox.Show("Error Processing item: " & oCellValue, "Title")
                    Continue For
                End Try
                'compare the filenames
                'Performs a text comparison, based on a case-insensitive text sort order
                'If strings equal returns 0
                If StrComp(oModelFileName, oRowFileName, CompareMethod.Text)=0 Then 
                    'Get the value of Item from the Parts List
                    'Row name needs to be case sensitive or use 1 for first 2 for second etc.
                    oCell  = oPartsList.PartsListRows.Item(j).Item("Item") 
                'Row name needs to be case sensitive or use 1 for first 2 for second etc.
                    'get the value of text in cell
                    Dim oItemValue As String
                    oItemValue = oCell.Value
                    
                    'Show the view label
                    oView.ShowLabel = True
                    'format the text first line
                    oStringItem = "<StyleOverride Underline='True' FontSize='0.35'> ITEM " & oItemValue & " </StyleOverride>"
                    'format the text second line
                    oStringScale = "<Br/><StyleOverride FontSize='0.3'>(Scale <DrawingViewScale/>)</StyleOverride>"
                    
                    'add to the view label
                    oView.Label.FormattedText =  oStringItem & oStringScale
                End If  
            Next
      End While
Next

------------------------------------------------------------------------------------------------------------

Later,

ADS

               

                

Reported Length

In one of my previous post I’ve shown you how to change length parameter format for steel shapes in Content Center (CC) so that assembly Bill of Materials (BOM) will have no trailing zeros and round up the value to a 1 mm increment.

On that post I gave you a bit of ilogic code that can change formatting of files you might have generated already which can come in hand and can be used with code injector.

At that time I didn’t realized that you might not use the assembly BOM to report your lengths but use the drawing Parts List so in this post we will look at doing just that.

If your company uses Parts Lists then you might be lucky and saved yourself a good couple of day’s work where you needed to copy all the default libraries to a custom read-write and then editing all the templates to report correct length parameters.

The Parts Lists can be formatted just like the parameter display and you can show/hide, trailing or leading zeros, units string or even change units to: in, mm, cm, m, ft, yard, mi, or microns.

Double click on your table or right click and choose “Edit Parts List...” either on the browser or graphical window.

Right click the quantity column and choose “Format Column...”. In the format column window you can specify a new name for the column, change text justification and most importantly you can change units formatting.

Click on “Apply Units Formatting” to activate the submenus. Now you can change trailing or leading zeros, change units type, units and precision. It can be configure to report a different measurement unit, to change decimal from "." to "," and you can choose if you need to have the units string displayed at all.

If you use the Materials List table style supplied with Inventor you will have to modify the Substitution tab in the format cell window. In the Substitution window you might have “Enable Value Substitution” and “When exists, use value of” PL. This is helpful for those that do Tube and Pipe where the reported parameter for pipe length is PL.

And of course there’s a catch. Your units will be rounded but you need to be careful because you can have it rounded up or rounded down. Both can cost you and rounding up an expensive material can be just as expensive as rounding down and not having enough to complete your design.

My settings will keep units to mm but will remove trailing zeros and set precision to 0 decimals. Most workshops will not need or manufacture to less than 1mm increments but this is for you to decide.

In this way you can keep the default formatting of CC and keep working with the out of the box libraries without the hassle of copying or editing them.

Later,
ADS

Documenting tube and pipe spools

+Paul Munford has been keeping me really busy so I didn’t had time to update the blog in 2 weeks… way too long.

Last time we were discussing reordering tube and pipe components, more exactly the lack of it and I have asked you to vote for this request on Autodesk Idea Station.

Meanwhile I have been trying to find some solutions on my own and I have taken a clean approach controlling my urge to search the internet for existing solutions.

In parallel I have been asking Autodesk to give us a way of converting a route (ipt) into a regular part that we can use outside T&P. At the moment its’ not possible but CAI from Adesk has given us a code that does 90 percent of the job done. However I am still testing this solution and it was all too big for a single video, single blog so it’s on for next time hoping it will become a valid solution for this problem.

First of all: What is a spool?

We call spool an assembly of pipe and fittings like elbows, flanges, tees, etc., usually terminated with flanges. Piping systems for process plants in general are commissioned into two stages: the pre-fabrication of pipe spools and the site installation. Some of the reason for pre-fabrication are limited space on site, weight of components, weather independent production, better quality, higher accuracy etc. On the down side they might not fit on site but all things considered spools are widely used throughout the industry.

My background is high quality, high purity water for medical, pharmaceutical and scientific industry so I don’t deal with spools at all but Autodesk is really slow at improving Tube and Pipe and I wanted to test the water and see what I can come up with. Decided to see what’s out of the box, ignoring ilogic and other vb scripts that could solve this mess.

In an ideal world you would have each spool as a separate run so that BOM and Parts List will indicate proper quantity but it’s not feasible to do ten thousands runs in a single T&P assembly. Keep in mind that due to its weight a spool can be just a flanged tee (think large diameters).

On this premises I would do the whole T&P in a single Run, mingle them all in and control the sizes by creating separate routes.

First solution: Design View Representations.

I bet you’re using this right now and there’s nothing new under the sun but I will present this anyway because there might be some nice tricks you’re not using at the moment.

I like to do my design view representations and level of details in a separate tab so open the assembly, locate the run and right click open. For simplicity I will call the assembly that contains the Tube and Pipe assembly “Main Assembly”.

TIP: You cannot create a design view from within the main assembly for the T&P assembly or any of its runs so if you want to modify design views you need open the files explicitly.

  TIP: Saving runs is only possible form the T&P assembly or any level higher but as long as they are both open you can modify the files and then switch back to the T&P assembly or any level higher (like the main assembly) and save the changes.

TIP: There is no Open option when right-clicking a route in the browser so if you need to open it you can select it in graphical window or the browser but right click on the graphical window to find the open command.

With the run open expand the Representations folder, right click the main view node and choose new. Click twice on its name to change it something more meaningful. Select your spool components and choose isolate from the right-click contextual menu.

TIP: To quickly choose parts at any level down bellow hold down SHIFT and in the right click menu choose Part Priority. Now you can select any part no matter how deep it is buried in the level tree.

TIP: Another way of isolating components is to select them and then hold SHIFT+right-click and choose invert selection to select all other where you can toggle Visible off.

In the drawing environment when placing the view select your design view previously created to bring in a and display just those components.

The main problem with this solution is the reported quantity and item number in the parts list.

While place a parts list for your view you will notice that all parts are shown but we can overcome this with a filter. Edit the parts list and choose Filter Setting, and in the Define Filter Item drop down menu choose Assembly View Representation. In the view representations choose the one you defined, click the green checkmark then OK for the Filter Settings window and OK again for Parts List window. Alternately instead of filtering for Assembly View representations you could filter for Ballooned Items. The parts list will be empty until you start ballooning your view and you will end up with same results only that you need to have balloons for each item you want to show up in the parts list.

You will notice that the quantity and item number will take into account the whole assembly and furthermore the item number might be out of sequence. You can use the renumber items function on the parts list but only if you detail each design view on its own drawing. The item override is drawing persistent so creating separate sheets will not work, and the changes on one sheet will modify all sheets so you will end up with weird sequencing or duplicate item number.

As long as you inform your fabricators that the quantity and the item number pertain to the whole project you might want to use this solution.

Second solution: iAssemblyes. (I can hear some eyes popping out).

Creating iAssembly members is another way of documenting the spools and with better results. Creating iassemblyes is not possible while editing the files from the main assembly and once again you need to open the files explicitly.

Right click on a run in the browser or graphical window and choose Open. On the Manage tab, Author panel click Create iAssembly. This will create configurations of the run where each member will be a separate file on disk. Right click on the Member column and notice that it’s marked as the filename column. Specify different names for your members but you can have same part number for all of them. Right click anywhere on row one, choose insert row and setup your part number and member/filename values. Click OK when you finished adding rows.

TIP: Use the Options button to setup sequencing and auto fill in for your member, part number values.

Once you close the iAssemlbly Author window you will notice a Table in the browser right under Relationships folder. This will contain all the children listed by the Member name. If you right click on the Table node you can choose:

-Delete (this will convert the ipart/iAssembly to normal)

-New (to create a new member)

- Edit table (this will edit the table inside Inventor)

- Edit via spreadsheet (will open in excel)

If you convert the T&P assembly or a run to iAssembly, the Edit table option is grayed out but all the rest will work and opening with excel will allow any operation like deleting a member.

TIP: If you want to edit the table inside Inventor you can click on Create iAssembly again from the Manage tab and it will bring up the table editor even though the option is grayed out in the browser contextual menu. Also, instead of creating the T&P files in the main assembly you can create another subassembly in between (a container if you will). The edit table will be available in here from the contextual menu or by double-clicking the Table node.

As a general rule if you have 3 spools then you need to create 4 members. The first member you will keep intact and it’s used to show and document the complete assembly while the other you will modify to show individual spools.

In order to modify a member alone without changing any other you need to activate the Edit Member Scope in the Manage tab, Author panel, Edit Factory Scope fly-out arrow.

Activate the second member and after selecting all the components that are not part of the spool choose Exclude from the contextual menu.

TIP: You can do that really quickly by choosing the spool parts and then hold down SHIFT + right-click and use Invert Selection. Now you can click Exclude from the contextual menu.

Do this for all spools and then save the file.

Open the drawing and place a view. In the Drawing View place dialog switch to Model State tab and choose the member you want to detail then click OK to place the view.

Placing  a parts list from that view will populate the table with only those components in the correct quantity as well. In the edit table window you can choose a different member to report by clicking the Member Selection button. Here you can also notice that Hide rows of zero quantity is checked. This is what hides the other members so keep it checked.

You can show the number if items by adding Item QTY to your list from the column chooser menu but DO NOT REMOVE QTY from the list while in here because the Parts List will show complete assembly again. Click OK in the Parts List Column Chooser and then right click the QTY column and select Column Width. Here enter a really small value like 0.1, click OK to accept and then Apply in the Parts List window.

This will hide the QTY column from the Parts List but depending on where QTY column was in the editor window you will see a double vertical line that you can drag left/right to show the column. Applying the changes will show QTY column in the editor window but not on the drawing.

TIP: You can zoom the editor window just like in any other program (adobe, web browser, explorer, office products) by holding down CTRL and spinning the mouse wheel up and down. This will make it easier to show the QTY column again.

So now we have proper items reported with a proper quantity but the item number is still out of sequence. Just like in the design view solution you can use the Renumber Items function in the table editor. Keep in mind that these are drawing specific so you need to detail each spool on a separate drawing rather than on separate sheets.

And this is it…. Are you still awake?

Like I have mentioned I am still experimenting with a different solution and I found a few bugs that need documenting. I hope to have it ready for next post.

Video to follow..

Later,

ADS.