Setting Material Properties Ansys

[nekojita]

I am trying to create a thermal model in Ansys with three layers of different materials. First I set the element material properties for the three different materials. Next, I am attempting to assign the element properties to each area using: Preprocessor>Meshing>Mesh Attributes>Pick Area. This is where the problem lies. After I have selected each area and applied element properties 1,2, and 3, I find that all three areas end up with the same material properties no matter how I select them.

I must be missing something obvious. Any help would be appreciated.

Thanks,

nekojita

 

[Drej]

First select the area you want to assign properties to using the ASEL command, then use AATT,mat,real,type where mat/real/type are the material/real constant/element type you want to assign to that area. The use ALIST to check that the correct mat/real/type have been assigned.

Cheers,

-- drej --

 

[nekojita]

Hi Drej,

Thanks for your reply. Your suggestion appears to use command line syntax which I less familiar with but will give it a try. Do you know why my method using Preprocessor>Meshing>Mesh Attributes>Pick Area does not work? This method was described in detail in the tutorial that I was following yet doesn't work.

Any thoughts?

Thanks,

Art

 

[cloche]

Art,

suggestion is to become familiar with command-line syntax because then you will be able to write your log files directly, which will open the door to "infinite" possibilities...
My idea, if the AATT command works for you while the menu method doesn't, is that you are making some mistakes in selecting the areas. Or you haven't defined the element type. As far as I know, elem type has to be defined prior to make any setting for meshing that can involve elements themselves, otherwise ANSYS will not know "with what" to mesh. The menu you recall is one of these: the program allows null-selection of real constant and section because not necessarily the elements use them, but if I'm not wrong, the other fields are mandatory.
I tried right now (usually if I have to do that I use components and then recall them, using log-file macros) with a very simple model made with v. 8.0 and it works !

Claudio

 

[nekojita]

Claudio,

Thanks for your comments, I will try working more with the command line. I tell you though, I really tried everything that I could think of last night trying to select those areas to apply the material properties. I thought that I had defined the element types for each area but maybe not. Possibly I defined the element type for the first area (thermal solid) but didn't apply the element type to the subsequent areas that I created. This would have left two of the areas undefined. In thinking back, I think that I thought that I had made a global definition of the element types when defining the element type for the first area. Does this make sense?

Art

 

[cloche]

Art,
I couldn't understand if you finally used the "ASEL-AATT" method or if you refer to the menu-method. Does ANSYS write some warning or error message in the output window when you try to select the areas? Or even with the command-line method, after issueing "ALIST,all" (warning: first use ASEL to limit selection to the areas you need, otherwise use "ALIST,area-min-number,area-max-number") you can see that the material assignment is wrong?
When you make a global assignment for elem type, this goes to all appliable entities in the database (for ex., if you give default elem type to PLANE42, lines will obviously not be affected), but you can still override this by making specific assignments, just like with the command you want to use. This should not affect material assignment, though...

You can also do that:
1- mesh with all areas using the same material
2- issue ASEL,s,area-num for the first area you want to modify (or ASEL,s,a-min,a-max for a sequence), or CMSEL,s,component-name if you have defined components made of the areas of the same type. The equivalent menu is Utility Menu -> Select -> Entities -> Areas -> ... or Select -> Select Components -> by name ...
3- issue ESLA,s to select all elements attached to the selected area(s). The equivalent menu is Select -> Entities -> Elements -> Attached to - Areas - From full
4- issue EMODIF,all,MAT,mat-number. The equivalent menu is Modeling -> Move/MOdify -> Elements -> Modify attrib -> pick all (as you already selected those you want to modify)-> Material.

This method DOESN'T change material default attribution to the AREAS themselves, but only to the ELEMENTS attached to the area. That means that, if for some reason you have to clear the area mesh and remake it, you will have to pay attention once again to elem / material attributes !!

Let me know if it works for you... BTW: which version of ANSYS are you using? Commands always remain the same, but menu paths not always... I'm presently refering to v. 7.0 / 8.0

Claudio

 

[nekojita]

Claudio,

Thanks again for your suggestions. Last night, I had a short time to experiment and thought that I would have it figured out but still it's a no go.

First I simply started with two rectangular elements. I created two element type numbers (plane55) and two material types.

From the mesh menu, I went to assign attributes (AATT) to area from the menu to the first element. The screen showed:

MAT Material number: 1
REAL Constant set number: none defined
TYPE Element Number: 1 PLANE55
ESYS Element Coordinate System: 0
SECT Element section: None defined

I clicked OK.

At that point, all looked good so I moved on to the second element and set the following:

MAT Material number: 2
REAL Constant set number: none defined
TYPE Element Number: 2 PLANE55
ESYS Element Coordinate System: 0
SECT Element section: None defined

Clicked OK.

When I went back to the Mesh menu and picked the element 1 area, I see:

MAT Material number: 2
REAL Constant set number: none defined
TYPE Element Number: 2 PLANE55
ESYS Element Coordinate System: 0
SECT Element section: None defined

The attributes of element 1 are now those of element 2. The properties of the last selection that I made are assigned to both areas.

Either I am in left field here still or am nearly there but am missing some little thing. Hopefully you can see which it is.

My version is 8.0. Also, how do I post files or screen captures in this forum. I don't see how to do that. It seemed that if I could send you my db file or post a screen capture it would be helpful.

Thanks,

Art

 

[cloche]

Art,

I don't know if we are allowed to post images or other attachments here, I suppose not...
Anyway, your description seems helpful: I think I understood what gets you confused!
What you see in the MENU when you open it by "Meshing > Mesh Attributes > Picked Areas > area selection" is the selection dropdown lists in the state in which they were the last time you used them, NOT in the state corresponding to the entity selected! Call ANSYS tricky and you will be perfectly right, but it's like that... ;-)
In fact, if you do exactly what you did in the example you describe, except that after setting the attributes for each of the two areas you control their effective properties by issueing the command "ALIST,all" in the command line, you will get this:

LIST ALL SELECTED AREAS.
NUMBER LOOP LINES AREA ELEM SIZE #NODES #ELEM MAT REAL TYP ESYS SECN
1 1 1 2 3 4 N/A 0.000 0 0 1 0 1 0 0
2 1 3 7 6 5 N/A 0.000 0 0 2 0 2 0 0

It's a bit difficult to read it HERE, but in reality it's clearer! You can see that the "MAT" property for area "NUMBER" 1 is "1" and "MAT" for area "NUMBER" 2 is 2, as desired!!! In my example, the ALIST command is issued before setting element size on each area, so "ELEM SIZE" is 0.000 for both. "AREA" is the size of the surface, not to be confused with the area number: it's N/A because no measurement has been performed (there's a command for that); #NODES and #ELEM are both 0 because the areas have not been meshed yet; "TYP" represents the element type and is 1 for area 1 and 2 for area 2. In fact, you didn't need to create a second copy of the same element type: just assign the different material and leave the elem-type selection on the only one you want.
Of course, you have none of these troubles if you rely on commands, but I agree it's a bit difficult if you're not used to...
I hope it works now!

c.u.!

Claudio

 

[nekojita]

Claudio,

Your the man. Thanks! I don't know if it's just me but I find The Ansys GUI arcane and archaic. It seems like a hybrid similar to the way AutoCad evolved. I hope that on newer versions, they can make a clean break to create a modern GUI.

On a couple of side notes, is it generally better to create adjacent areas separately or to create a larger area and split by setting up keypoints?

Also, I had trouble reading in an IGES file exported by Solidworks. It didn't look anything like the SW drawing when I brought it into Ansys. Any thoughts?

Thanks,

Art

 

[cloche]

Art,

I'm glad we've found the solution for your problem! Yeah, ANSYS have a "very strange" (!!!) GUI, with a VERY steep learning curve, but once you get used to it I think it's one of the most powerful and reliable FEA software ever thought and made by human beings!! If you didn't need to model directly in ANSYS, you could use Workbench interface, that loks and feels like the one of the most common CAD softwares, such as SolidWorks. In v. 9.0, to which fortunately my company will upgrade within short times, this Workbench has been further improved... I know ANSYS' plans are to converge to Workbench (but probably this will mean loosing forever the modeling capabilities... You then will have to have a CAD on your workseat + ANSYS...).

To your question: I generally prefer to have separate areas instead of dividing them. I divide areas (or, in general, entities) only if the model given to me by the designers proves not to be 100% compatible with the mesh I want to obtain (for example, mapped or sweep type...).

IGES importing is also tricky: you can only do this OUTSIDE of any processor, i.e. when you are in your model, issue a "FINI" (abbreviation for "FINISH") in the command line to exit any processor, then go to File > Import > IGES...
Moreover, it sometimes give errors if path+name is longer than I don't remember how many bytes, or if the filename / path contains spaces (e.g. "\Documents and Settings\".
If your errors are not of this type, i.e. the entity translation starts and finishes but you can't get the correct geometry, then this may be due to tolerances: too stiff or too loose I don't know (we should see your model). You can try to adjust the option "merge coincident keypoints" (if it's on, turn it off and see if at least the surfaces get imported - the solid will probably not because of boundary representation incoherence). If, instead, you get geometry without any warning or error message in the output window, but you can only see wireframe lines in the graphical window, simply give "/RESET" in the command line and then Plot > Replot.

Ciao

Claudio

 

[nekojita]

Claudio,

Thanks again for your response and support. I'll get there, but as you say, the learning curve is steep. At a conference I was at in January (SPIE) several researhers that I conferred with made the same comment about the learning curve but also commented that in end it was worth the 'climb up the mountain' as one fellow put it. Especially so in the area of coupled fields.

Best Regards,

Art