iLogic to Access Material Information

[Anonymous]

I'm not sure if this is possible through the API or not, but there are a lot of smart folks on here so let's give it a shot. I would like to make a rule that will take information from the material "Descriptive Information" "Comments" line and put it in the Stock Number iProperty. We have a large library of custom materials and I want to put the raw material stock number in the comments field then use iLogic to extract it and apply it to the Stock Number whenever the material is changed.

[HermJan.Otterman · Accepted solution]

Hello Dale,

Yes you can.

Here is an iLogic rule that does that.

 Dim oPartDoc As Inventor.PartDocument = ThisDoc.Document
  Dim oRawMatNo As String = oPartDoc.ActiveMaterial.Item("physmat_Comments").Value
  MsgBox(oRawMatNo)
  iProperties.Value("Project", "Stock Number") = oRawMatNo

 (delete the MSGbox line)

[Anonymous]

Exactly what I needed, thanks!

[Anonymous]

Currently I am using the above rule for my active materials which works very well, but I was wondering if there is a way to access an inactive material comment based on a multi-value text parameter that matches an inactive material name.

[Anonymous]

---

Hi

Is there a list of all the names from the material information properties?

  Dim oRawMatNo As String = oPartDoc.ActiveMaterial.Item("physmat_Comments").Value

For example: physmat_Comments is for the Identity Tab -> Comments box

                        physmat_Manufacturer is for the Identity Tab -> Manufacturer

How to access in the Physical Tab the boxes like Name, Description, Keywords, Source etc.

Thanks

---

[HermJan.Otterman]

try:

Physmat_Comments

Physmat_Cost

Physmat_Keynote

Physmat_Keywords

Physmat_Label

Physmat_Manufacturer

Physmat_Mark

Physmat_Model

Physmat_Type

Physmat_URL

Appearance and Physical tabs

oPartDoc.Activematerial.PhysicalPropertiesAsset.item(“.....”)

structural_density

structural_behavior

etc..

Generic_self_illum_color_temperature

Generic_self_illum_filter_map

generic_self_illum_Luminance

Generic_Transparency

Etc, 

(do a for each item and list the names….)

[HermJan.Otterman · Accepted solution]

pHysical ...

        Dim oPartDoc As PartDocument =  ThisDoc.Document

        Dim ActiveMat As Asset = oPartDoc.ActiveMaterial
        'list all Identity AssetValues:
        For Each oAssetValue As AssetValue In ActiveMat
            MessageBox.Show(oAssetValue.Name)
        Next

        Dim ActiveApperancePhysical As Asset = oPartDoc.ActiveMaterial.PhysicalPropertiesAsset
        'list all Appearance and Physical
		msgbox("")
        For Each oApperancePhysical As AssetValue In ActiveApperancePhysical
            MessageBox.Show(oApperancePhysical.Name)
        Next

[Anonymous]

Thank you very much @HermJan.Otterman !

That's exactly what i was looking for. Unfortunately I can't find where to accept as solution!

Best regards

j

[HermJan.Otterman]

great that you found your solution.

the accept is only if you created the initial question.

thanks

[HermJan.Otterman]

with this code you go through ALL material in you project file:

Dim AssetLibs As AssetLibraries = ThisApplication.AssetLibraries
Dim AssetLib As AssetLibrary
For Each AssetLib In AssetLibs
	Dim oMaterialAssets As AssetsEnumerator = AssetLib.MaterialAssets
	Dim oMaterial As MaterialAsset
	For Each oMaterial In oMaterialAssets
		msgbox(oMaterial.displayname)
	Next
Next

 where the messagebox is, you can put the code from the previous answer to get to the properties

[Anonymous]

This is great information...

Perhaps I'm missing it here, but what I really need is to pull the Appearance Name associated with a material. Material/Appearance/Information/Name

[bradeneuropeArthur]

Public Sub asse()

Dim a As Application
Set a = ThisApplication

Dim oAsset As Asset
Dim oAssets As Assets

Set al = a.AssetLibraries.Item("YOUR MATERIAL LIBRARY NAME")

Dim m As MaterialAsset
For Each oAsset In al.MaterialAssets
If oAsset.DisplayName = "YOUR MATERIAL" Then
Debug.Print oAsset.Name
Set m = a.AssetLibraries.Item("YOUR MATERIAL LIBRARY NAME").MaterialAssets.Item(oAsset.Name)

MsgBox m.AppearanceAsset.DisplayName
MsgBox m.DisplayName
End If

Next

Regards, 

[RoyWickrama_RWEI]

I explored your posting. Great help. However, my need is to retrieve mostly the material of the current part document. Like to retrieve other data Other data (appearance) as well.

[Anonymous]

Hi!

I need some help for the following problem. I would like to get information about Material Editor / Physical / Name.

I will create a code when i will filter the surface treatment. When i choose the "steel", i can select between black oxided, nickel plated, ... When i choose the "aluminium", i can select anodized.

I need this Physical name, but i can't know how i get this parameter.

Tthanks

[ic198]

Hi Herm Jan,

Do you know how to access the Material Description on the Identity tab? I don't see it on your list, and this thread suggests it might not be available?

https://forums.autodesk.com/t5/inventor-forum/material-description-as-custom-iproperty/td-p/6913143

Thanks for your help

[Anonymous]

Hello,

Unfortunately I can replay at now.

I use the following code to list the physical information. And I can't find the Name of Physical. I can't find this in API table.

Dim oPartDoc As Inventor.PartDocument = ThisDoc.Document

Dim oActivePhysical As Asset = oPartDoc.ActiveMaterial.PhysicalPropertiesAsset
MessageBox.Show(oActivePhysical.Name)
For Each oPhysical As AssetValue In oActivePhysical
MessageBox.Show(oPhysical.Name, "Azonosító")
Dim oPhysMat As String = oPhysical.Value
MessageBox.Show(oPhysMat, "Érték")
Next

[ic198]

Thanks @Anonymous 

@johnsonshiue, do you know why the material description is not available, and seems to be the only property that isn't available? I want access to it because it is easy to update, whereas changing the Name property creates a new material

Thanks

ic198

[ppolcynBNVFN]

Is there a way that I can copy the comment from the message box to my clipboard when it pops up? Right now it is unselectable.

[Curtis_Waguespack]

@ppolcynBNVFN, you can use an Inputbox rather than a message box, or better yet use the logger so you don't need to click OK , 9000 times.

Hope that helps.

Dim oPartDoc As Inventor.PartDocument = ThisDoc.Document

Dim oActivePhysical As Asset = oPartDoc.ActiveMaterial.PhysicalPropertiesAsset
	InputBox("", "Active Physical Name", oActivePhysical.Name)
For Each oPhysical As AssetValue In oActivePhysical
	InputBox("", "Azonosító", oPhysical.Name)
	Dim oPhysMat As String = oPhysical.Value
	InputBox("", "Érték", oPhysMat)
Next

'show ilogic logger
ThisApplication.UserInterfaceManager.DockableWindows.Item("ilogic.logwindow").Visible = True

Dim oPartDoc As Inventor.PartDocument = ThisDoc.Document

Dim oActivePhysical As Asset = oPartDoc.ActiveMaterial.PhysicalPropertiesAsset
Logger.Info("Active Physical Name")
Logger.Info(oActivePhysical.Name)
For Each oPhysical As AssetValue In oActivePhysical
	Logger.Info("Physical Name")
	Logger.Info(oPhysical.Name)

	Dim oPhysMat As String = oPhysical.Value
	Logger.Info("PhysMat")
	Logger.Info(oPhysMat)
	Logger.Info("")
Next

[ppolcynBNVFN]

That works perfect. I just used an input box as I just need one property. Thanks!