Best way to duplicate part/drawing?

[Anonymous]

So, I'd like to make a derivative part and copy the drawing.  Save as a copy sounds good but I want the drawing and part to both get copied.  Pack and Go seems like overkill.  ANy advice?

Thanks

[Anonymous]

https://forums.autodesk.com/t5/inventor-general-discussion/change-part-reference-in-drawing/td-p/376...

[CCarreiras]

HI!

1. Close files in inventor
2. Copy both in windows folder
3. rename file names and Part Numbers
4. Rebuild the links (Part reference).

Open the solid, and select "Open drawing and indicate the correct drawing document to reactivate the links and references)

[karthur1]

If you were using Vault... that is called Copy Design.  Makes it really easy and it links the copied files for you.

Another way to do it is with the Design Assistant.  Open the idw and change the action to Copy.  Also change the other columns also that need to be changed.  Save it then open the new file.  The idw should already link to the correct files.

Kirk

[Mark.Lancaster]

Another option is to use iLogic Design Copy (http://synergiscadblog.com/2014/09/23/copy-files-easily-with-ilogic-design-copy-even-without-ilogic-...

[rhasell]

Hi

My 2 cents worth.

Don't use Windows explorer to copy/rename your files. This used to be the only way to do this a few years back, but there are better tools available now.

Depending on the quantity of files you need to process, will determine what method you use.

(You have already answered your question with the link supplied.)

The easiest it to do the "save as" method. (But can become tedious if you want to do a lot of files at one go)

- Start with the Assembly

- Progressively "Save and Replace" each sub assembly/part

- The from each part, replace any derivatives.

Then Open each drawing/s and do a "Save as" for each one. (If multiples)

- For each new drawing use the "Manage/replace model reference" and select the 'New' Part/assembly.

The next method is to use the Design assistant

This works really well for multiple files and assemblies

I Personally have not used it for the corresponding drawings, so I still do the drawings manually, as above.

The last one is to use the iLogic design copy method.

This one is really cool, and works a treat, but it might not give you exactly what you want, as you still have to quite a bit of leg work to fix, part numbers and drawing names and numbers.

You only have the option to add a Prefix or Suffix to the file names, but all links and part numbers are updated, including 3rd party files.

I use all three methods, but the most common one is the basic "Save As" (Method one)

I got some iLogic code a while back (From the forum) which changes the derived component reference. This will be a requirement, as there is no easy way to do it via the "Save as " method.

Hope this makes sense.

[Anonymous]

The link I found was exactly what I was looking for.  I'm a SW convert, so there, save as renames in session which is very handy, but you can also change the model reference.  Changing the model reference is actually a fiarly cumbersome process in SW, so Inventor is considerably nicer there.  For now, save as, the change reference will do it.  I appreciate the other options and will try those out.  Thanks!

[rhasell]

Hi

Here is a piece of code which will help a lot.

Create an external rule, so that it is always available. As you progress, your arsenal of tools will grow, and its easy to access everything if you place them in an iLogic form.

I cannot take credit for this, I can't remember who wrote it.

I called mine "Replace derived component"

It will only work if the two masters (Source components) are/were the same I.E have changed via a "Save as"

Dim oDoc as Document
oDoc = ThisDoc.Document
Dim oRefFile As FileDescriptor
Dim oOrigRefName As Object     

For Each oRefFile In oDoc.file.ReferencedFileDescriptors
'get the full file path to the original internal references
oOrigRefName = oRefFile.FullFileName

'present a File Selection dialog
Dim oFileDlg As inventor.FileDialog = Nothing
InventorVb.Application.CreateFileDialog(oFileDlg)
oFileDlg.InitialDirectory = oOrigRefName
oFileDlg.CancelError = True
On Error Resume Next
oFileDlg.ShowOpen()
If Err.Number <> 0 Then
Return
ElseIf oFileDlg.FileName <> "" Then
selectedfile = oFileDlg.FileName
End If

'replace the reference
oRefFile.ReplaceReference (selectedfile)     
InventorVb.DocumentUpdate()
oOrigRefName = ""                                        
Next

iLogicVb.UpdateWhenDone = True

[Anonymous]

Man, that looks like Swahili to me.  I'm very excited to get into the API, but not sure I'm going to get to it soon.  I assume that's VBA?  Thanks

[rhasell]

Hi

It's not that bad, Yes I guess Swahili pretty much sums it up. but when you start getting into iLogic a whole new world opens up for you. I makes you feel like a programmer, but you aren't.

I think it's close to VBA, most of the commands and sequences work the same, but don't stress, you don't have to get into the API and there is heaps of help on the forum. (Most of my rules developed from snippets found on the web, I then combine and changed them to suit my needs) Where possible, I share them and give credit to the author.

Start small, not like one the guys in the office who decided to automate an entire model and drawing set at his first attempt, before even learning Inventor, needless to say he is still whimpering in the corner.

iLogic has brought it to the user, and it separates Inventor from all the others.

[Anonymous]

---

@karthur1 wrote:

If you were using Vault... that is called Copy Design.  Makes it really easy and it links the copied files for you.

Another way to do it is with the Design Assistant.  Open the idw and change the action to Copy.  Also change the other columns also that need to be changed.  Save it then open the new file.  The idw should already link to the correct files.

Kirk

---

This is the only answer you are looking for. The rest are crude or old ways that have a lot more manual work to complete.

In order of ease of use and preference in my experience I would suggest these (high to low with gaps indicating difference amounts):

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

1) Vault (Copy Design)

2) Design Assistant

3) Save as a copy and relink new model

4) Copy in windows and relink

5) Custom code or ilogic.

[ales.kadlec]

Hi,

I tried your procedure with design assistant.

I have similiar problem - I have part and drawing that I want to change, but also preserve.

When I copy part and drawing and set them with same name, it won't change the source of drawing - it is still under old part. Some advices how to fix it? Shall I better use vault?

[SBix26]

If they have the same name, how is Inventor going to distinguish between them?

Give us more detail about your workflow and desired outcome-- PartA.ipt with drawing PartA.idw, in folder X under project Y.  Now what?  Copy them where?

---

Sam B

Inventor Pro 2024.1 | Windows 10 Home 22H2

[johnsonshiue]

Hi Ales,

I could be wrong but I think Design Assistant should just work for your purpose. If possible, please share an example that illustrates the behavior. I would like to understand it better.

Many thanks!