cancel
Showing results for 
Search instead for 
Did you mean: 
cancel
Showing results for 
Search instead for 
Did you mean: 

Community Tip - Learn all about PTC Community Badges. Engage with PTC and see how many you can earn! X

Material ID

ChiselnMallet1
12-Amethyst

Material ID

Hello,

 

I am having trouble finding the material ID for use in a note.  I have created a new parameter in my material called "SPEC" that I'd like to use in my note.  But I cannot find where to get the MTRL_ID

 

Thanks for any assistance.

1 ACCEPTED SOLUTION

Accepted Solutions

Hi, Here is the way I do it.

If your user defined parameter in material is called SPEC then to reuse that as a note the I pull the material parameter into a model parameter. It might work by just doing &material_param("SPEC") but I would create the relation to make SPECIFICATION=material_param("SPEC") then the note is &SPECIFICATION. As it happens I also have IF else statements to show the note as unassigned if the material has not been assigned to the part.

View solution in original post

13 REPLIES 13

Is your material ID in the parameter list?  If it is copy the exact name of the parameter.  In your annotation type "&" then the parameter name. (e.g. &MTRL_ID).


There is always more to learn in Creo.

Hi, Here is the way I do it.

If your user defined parameter in material is called SPEC then to reuse that as a note the I pull the material parameter into a model parameter. It might work by just doing &material_param("SPEC") but I would create the relation to make SPECIFICATION=material_param("SPEC") then the note is &SPECIFICATION. As it happens I also have IF else statements to show the note as unassigned if the material has not been assigned to the part.

BenLoosli
23-Emerald II
(To:Roy_Crerar)

Segment from one of my material files:

{
Name = PDM_NAME
Type = String
Default = 'A36 STEEL'
Access = Full
},
{
Name = DESCRIPTION1_U
Type = String
Default = 'UNS K02599, STEEL'
Access = Full
},
{
Name = DESCRIPTION2_U
Type = String
Default = 'A36 STEEL'
Access = Full
},
{
Name = DESCRIPTION3_U
Type = String
Default = 'A36 ST'
Access = Full
},

 

Segment from my Relations:

/*** SET MATERIAL PROPERTIES ***
IF PTC_MATERIAL_NAME=="UNASSIGNED"
MATERIAL="UNASSIGNED"
MATERIAL_DESC1="NO MATERIAL ASSIGNED"
MATERIAL_DESC2=""
MATERIAL_DESC3=""
ELSE
MATERIAL=material_param("PDM_NAME")
MATERIAL_DESC1=material_param("DESCRIPTION1_U")
MATERIAL_DESC2=material_param("DESCRIPTION2_U")
MATERIAL_DESC3=material_param("DESCRIPTION3_U")
ENDIF

 

Once a material is set, the relations pull the parameter information in.

 

In the model file, we have a saved annotation (material_std_note):

&MATERIAL_DESC1
&MATERIAL_DESC2
&MATERIAL_DESC3

 

This gets pulled into the drawing.

Why are there 3 different material descriptions?

This is a bad example because A36 is a common material. We use some materials that need the 3 lines for their descriptions to get fully defined. If a description line is blank, it will be blank on the drawing.

Is it possible to put a parameter table in the .mtl?  I notice the syntax the beginning of the file is different from the restricted value parameter files.

 

ND_RelParSet_K01 = { ***from .mtl first line

 

ND_ParamDefArr_K01 = { ***from restricted value file first line

and the parameter table line is

ND_ParamTable_K01 = {

 

Wondering if a table in the .mtl file needs to be something like "ND_RelParTable_K01"?

 

 

 

 

 

I was having trouble defining the material's ID in the part file itself.  But eventually found that I didn't need the ID to call it.  That the &material_param("xxxx") method called the active material.

 

Thanks you for your reply!

Material ID could be found by adding a material parameter to relationships.

Creo will prompt a list with all available material

select material by name

Creo replaces it with internal ID

Can you please provide syntax/example to it for understanding it better. 

BenLoosli
23-Emerald II
(To:SS_10854866)

Log into Creo and go to File-Prepare and then select assign material. You can create a blank material file that will give you the syntax for the material files. In the other thread, I pasted a full file for 7075-T6.

The Creo online help has a section on the Material Library.

 

You could start from drawing relationships as well as from model relationships.

Material-ID number could be copy-paste to be used on any note.

 

I tried this method

1. Write material= in relations 

2. Go to parameter 

3. Select PTC_MASTER_MATERIAL

 The relation is successfully added but the material ID is not displayed. Can you please let me know where the material ID will be displayed?

Hi,

For me it shows up on pos 6 (see attached screenshot). E.g. I added the IACS electrical value.

I didn’t try with PTC standard material. Works perfect for materials assigned by me.

Our Standard parts always have materials assigned so I am not able to check out of the box behavior.

Did you follow the steps on drawing?

Go to relationships Add new variable Add parameter > search in “material” > select your material from list > add attribute parameter from available parameter list. After “add selected” and close parameter selection window, MTL ID should show up in relations editor line.

Top Tags