iLogic

[matheuspalha71]

Hello,

New here, first post.

I apologize in advance for using an online translator

I went through all the research I could think of, but I couldn't find exactly what I was looking for. I hope you can help me.

I would like to be able to enumerate the parts in which model in order to be able to attach the number in the drawing automatically

example: when we open a modeling model, '' Part1 '' appears and provides the sequence '' Part2 '', '' Part3 '' ... and so on

I would like to be able to enumerate separately on some property, such as the stock number in the modeling sequence, to be able to automatically attach to the parts list

Thank you very much in advance

[Anonymous]

Are you wanting to balloon parts on the drawing through iLogic? It sounds to me like you are wanting to assign each part a number to then label those parts with that number in the drawing. This functionality is already built into parts lists and the balloon feature. If automated ballooning is the goal there is functionality for it, however it is not a small task and takes place in the drawing environment. If I misunderstood please re-direct me.

Hope this helps!

[matheuspalha71]

Yes, but in a detail of an assembly, it takes the order according to what I added in the assembly right? I would like him to place the order according to what I modeled, you know? can i send a photo to try to explain better

[Anonymous]

So if you model part A and then part B, but create an assembly by placing B first then placing A, you are wanting to re-order the parts list A to B? What is your reason for wanting the parts in order of when modeled as opposed to the standard ordering? I'm just trying to get a clearer picture so I can tailor a suggestion accordingly. I also do not want to suggest adding complexity to your workflow in the form of iLogic if there is an out-of-the-box functionality that will work for you. You can also re-sort according to part number, description, etc. for fields that are shown in the parts list

[matheuspalha71]

So, I am a competitor of the knowledge Olympics, of the integrated manufacturing occupation, and competition requires this type of task, and so I'm trying to facilitate the process, so I don't have to worry about adding the parts in order in the assembly, you know?

[WCrihfield]

Perhaps adding a new custom column to the Parts List that shows the CreationDate or LastModified date, then re-order according to that colmn?  The if necessary, delete that column again?  This might be a little complicated to do with iLogic, but is propably doable.  What do you think?

[Anonymous]

This is what I was going to suggest, but I do not believe that the API functionality is there for working with parts lists through code. I know you cannot filter them via the API so I assume this to be the case, though I may be wrong.

[WCrihfield · Accepted solution]

Try this iLogic code. It works for me.

Dim oDoc As DrawingDocument = ThisDrawing.Document
Dim oPartsList As PartsList = oDoc.Sheets.Item(1).PartsLists.Item(1)
Dim oPropSet As PropertySet = oDoc.PropertySets.Item("Design Tracking Properties")
Dim oPropSetID As String = oPropSet.InternalName
Dim oPropID As Long = oPropSet.Item("Creation Time").PropId
Dim oCDColumn As PartsListColumn = oPartsList.PartsListColumns.Add(PropertyTypeEnum.kFileProperty, oPropSetID, oPropID, oPartsList.PartsListColumns.Count, False)
oPartsList.Sort(oCDColumn.Title, True)
oPartsList.Renumber
iLogicVb.DocumentUpdate
oCDColumn.Remove
iLogicVb.DocumentUpdate

I hope this helps.
If this solves your problem, or answers your questions, please click 'Accept As Solution".
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Here are a few of the ideas I like.
If you agree, please vote for them, so they might get implemented.

• Options to format contents of MessageBox, InputBox, and InputListBox Click Here
• Ability to fully constrain and dimension to the edjes of images within drawing title block sketches, SketchedSymbol sketches, other drawing sketches, and assembly sketches Click Here
• Save section view status in DesignViewRepresentation, so it can be used in drawing view Click Here
• Add SolidBodies folder to iLogic Rule Editor Model Tab Click Here
• Convert all views to Raster before autosave stores to 'OldVersions' folder Click Here
•  

[Anonymous]

Sweet, I didn't know this functionality was there! Good to know

[matheuspalha71]

That's exactly what I was looking for !! Thank you very much, I am very grateful! His rule was fundamental to help me think of others !!