I would like to know if there is any way of outputting a .dxf automatically when you check in an idw file to vault?

We have setup the option to output a dwf file to a specific folder so our shops can open and view parts and assemblies, but have yet to figure out how to do this with a dxf file so that our part files can be converted and saved to a folder for our machine shops to be able to access them on their own.

Currently we have to manually do this by selecting the "save copy as" option and then navigate to the folder on our network select to output the file as a dxf and then save it.

Any help on this would be greatly appreciated.

Thank you,

Darrin S.

This may help you

viewtopic.php?f=34&t=11249

Thank you PeterCharles for you reply but will this work with standard .ipt files or must they be sheet metal parts?

We mainly will be using this to output to a water-jet & a plasma cutting machine to cut from sheet metal, but most of the parts we will be outputting are standard .ipt files and not a sheet metal .ipt so no bends etc...

Also if anyone knows how to automate this function from an .idw file, that is the method that we would prefer to use.

I'm confused, you're cutting sheet metal??
Sheet metal parts don't need to have bends, lots of mine are just profiled flat plates, we just regard them as sheet metal parts because the production process is to cut them from sheet metal by laser.

I understand how this might be confusing, and I apologize for not explaining in a little more detail about what we face in this scenario.

The thing is that any part that has been created was done as an standard .ipt even if it is cut from a flat sheet of material. We could convert the parts to sheet metal .ipt files but this process would be overwhelming to say the least just due to the number of parts that we are talking about. And looking at your add-in that you recommended it looks like it would do exactly what we would want, but the only issue is that I cannot use it unless it is an assembly or a sheet metal .ipt file.

Example: A part is drawn in Inventor as a standard .ipt file and then an .idw is created for the part. Then with the .idw open we then have to select "save copy as" then navigate to the file location on our local network and then export the file as a dxf. Which in itself gets pretty monotonous. Which is why I am looking for some way of automating this output from the .idw file. I hope this explains the predicament a little better.

I understand your problem.

1) are you looking to put the DXF in the vault along with the IPT and IDW?

2) if yes that's beyond me to do automatically. I've searched for help on an IV macro to automatically check stuff back into the Vault but without success. Currently no one seems to be able to explain how to do it, something I'm at a loss to understand since you have access to the API's of both IV and Vault, but here seems no way for them to talk to each other.

3) if you have a set place into which the DXF must be filed then it would be possible from a IV macro (I think) that you run after saving the IDW. I assume the DXF of the IDW will be model geometry only?

4) based on you having a lot of IPT's already in the vault, could you consider checking out a complete directory, and converting them to Sheet Metal and creating Flat Patterns from a macro. Ah, snag, you need to manually select the surface for the flat pattern to be sure you get the right result. -- forget this one!

I think you're back to (3) and if there are a lot of places you might wish to save the DXF, then you might not save much time as you'll still have to select the directory manually.

Maybe someone else may have some suggestions.

Here is an example of one the parts that we might work with.

This a flange that would be cut from a sheet of 1/4" thk sheet of mild steel.


We will be putting the DXF's into a single directory on the network. We don't have to have it done automatically if I can use a macro to selectively output from idw's to dxf to the specified directory when we wish to have the parts made. However it would be nice to have the dxf's created in the directory after the idw is saved and then uploaded to vault. Pretty much like the option that is in inventor to output a dwf file in a selected directory when the file is save and checked into vault.


I do appreciate all of the input you have provided and I hope there is something out there that could make this work.

I'll have to sleep on it

Good night!

If you have iLogic (Included in Inventor 2011) it contains the code below. You could set the trigger to run when you save the file (it won't do it on check in to Vault though).

This might be one way to get there. Hope this helps!

iLogic code below.


' Get the DXF translator Add-In.
Dim DXFAddIn As TranslatorAddIn
DXFAddIn = ThisApplication.ApplicationAddIns.ItemById("{C24E3AC4-122E-11D5-8E91-0010B541CD80}")
'Set a reference to the active document (the document to be published).
Dim oDocument As Document
oDocument = ThisApplication.ActiveDocument
Dim oContext As TranslationContext
oContext = ThisApplication.TransientObjects.CreateTranslationContext
oContext.Type = IOMechanismEnum.kFileBrowseIOMechanism
' Create a NameValueMap object
Dim oOptions As NameValueMap
oOptions = ThisApplication.TransientObjects.CreateNameValueMap
' Create a DataMedium object
Dim oDataMedium As DataMedium
oDataMedium = ThisApplication.TransientObjects.CreateDataMedium
' Check whether the translator has 'SaveCopyAs' options
If DXFAddIn.HasSaveCopyAsOptions(oDocument, oContext, oOptions) Then
Dim strIniFile As String
strIniFile = "C:\temp\dxfout.ini"
' Create the name-value that specifies the ini file to use.
oOptions.Value("Export_Acad_IniFile") = strIniFile
End If
'Set the destination file name
oDataMedium.FileName = ThisDoc.PathAndFileName(False) & ".dxf"
'Publish document.
DXFAddIn.SaveCopyAs(oDocument, oContext, oOptions, oDataMedium)
'Launch the dxf file in whatever application Windows is set to open this document type with
i = MessageBox.Show("Preview the DXF file?", "Title",MessageBoxButtons.YesNo,MessageBoxIcon.Question)
If i = vbYes Then ThisDoc.Launch(oDataMedium.FileName)

_________________
Jonathan Landeros
Applications Engineer
KETIV Technlogies
Blog: www.inventor-tales.blogspot.com

Should

be

I could be either. iLogic uses VB.NET syntax instead of VB6 so the "Call" keyword is optional.

_________________
Brian Hall
"Good enough" isn't good enough for me.
Follow me on Twitter @Hallmanac

Ah, I'm on 2010 so don't have iLogic and am used to VBA/VB syntax.
(So I can't view the attached files either)

I appreciate all of the input on this issue. We will make a go at all of the recommendations and see where we are at. If I find another solution to this problem I will update on this post.

Thank you again, and wish me luck.

Glad I came across this, it's just what I was after.