Manual modification of thickness and nodal eccentricity to simulate wear

Solution Partner Experimenter Solution Partner Experimenter
Solution Partner Experimenter

Hello community,

Someone knows how to manually edit the thickness and nodal eccentricity of cshell elements.

I want to simulate wear by erosion or corrosion in pressure vessel. I'm interested in overwriting the automatic application of thickness by a manual definition, so I would like to keep the top surface continuous and apply nodal eccentricity in the botton surface  in order to represent internal wear and evaluate shell stresses and bending stresses and  estimate the amplification factor by wear effect.

 

For example:
Node i 102 thickness 6.01 eccentricity -0.34.

To import or read an .exel, .dat or .txt

Someone knows how I can do it.

 

Thanks in advance

5 REPLIES 5

Re: Manual modification of thickness and nodal eccentricity to simulate wear

Phenom
Phenom

Hi RMS,


if you want to modify the shell thickness in NX Simcenter to provide thickness reduction, try to use expressions for thickness reduction and offset as an attempt.


In property PSHELL use for default thickness a reduction factor as the expression: RATIO_OF_REDUCED_THICKNESS = 0.9 (or others)

RATIO_OF_REDUCED_THICKNESS = 1.00 means no reduction
RATIO_OF_REDUCED_THICKNESS = 0.1  means "remaining thickness" is 0.1 * given thickness (here 286 mm)

------------------------------------------------------------
 
              MESH COLLECTOR INFORMATION
 
------------------------------------------------------------
 
 
MESH COLLECTOR INFORMATION
    Name                                : SHELL_t286mm
    Type                                : ThinShell

     ==== Physical Property                   
    Shell Property                      : SHELL_t286mm
        Name                                : SHELL_t286mm
        Type                                : PSHELL
        Label                               : 1

         ==== Materials                           
        Plane Strain                        : false
        Material 1                          : CastSteel
        Use Material 1 for Material 2       : true
        Use Material 1 for Material 3       : true
        Material 4                          : (none)
 
        Default Thickness                   : 286*RATIO_OF_REDUCED_THICKNESS mm (257.4)
        Bending Coefficient of Inertia Ratio: 1
        Transverse Shear Thickness Ratio    : 0.833333
        Nonstructural Mass                  : 0 kg/mm^2
        Fiber Distance, Z1                  : Not defined
        Fiber Distance, Z2                  : Not defined


Then you can reduce shell thickness in  a convenient way by modifying the expression.

 

For the offset it's the same but the formula is more complicate:
If the shell thickness is reduced to e.g. 90 % and top surface is the direction of offset orientation you have to move element in positive direction about normal direction of mid-surface of  (sheet) body, try that:

MESH INFORMATION
    Name                                : SHELL_t286mm(1)
    Type of mesh                        : 2D Mapped
    Export Mesh to Solver               : True
...
     ==== Shell Offset                        
    Shell Offset                        : (1-RATIO_OF_REDUCED_THICKNESS)/2*286 mm (14.3)

     ==== Material Orientation                
    Material Orientation Method         : Orientation Angle
    Orientation Angle                   : Not defined

     ==== Thickness                           
    Thickness Source                    : Physical Property Table
 
    Use Element Associated Data         : true
    Layer                               : 1
 
    MESH COLLECTOR INFORMATION
        Name                                : SHELL_t286mm
        Type                                : ThinShell

...


I guess you have to modify all of your shell definition properties, and offset is defined in  "Mesh associated data" for every single mesh.

You can check the success in NX Simcenter 3D by using

 

MESH Display => 2D => "[x] Element Thickness and Offset"


May be it helps. Best wishes, Michael



| Production: NX10; Development: VB, TCL/TK, FORTRAN; Testing: NX12 | engelke engineering art GmbH, Germany | 2019-07-08
| Kudos for good posts! And if my post answers your question, please mark it as an "Accepted Solution". Kick Off (2015-09-14)On the Map (2016-10-21)1st Gear 2018 (2018-02-19)5th Birthday! (2018-02-25)Popular (100, ‎2018-10-30)Prolific (100, 2019-02-27)Philosopher (500, ‎2019-02-28)Problem Solver (50, 2019-06-25)

Re: Manual modification of thickness and nodal eccentricity to simulate wear

Solution Partner Experimenter Solution Partner Experimenter
Solution Partner Experimenter

Thanks Michael,

 

But, I can not solve it yet

 

I need to apply a measurement thickness by table field , this step is OK,
By default, Which variable or expression are used to storage the thickness information defined by table field definition?, I don't know which is the name of the variable.

 

I'm trying to use the default thickness expression included into the expression list. But I can't.

 

Please, could you upload a short video explaining the right form? in order to simulate this.

 

Thanks in advance

 

table field thikness - table field.JPGtable field thikness - 0.JPGtable field thikness.JPGtable field thikness - 2.JPGtable field thikness - 4.JPGtable field thikness - 5.JPG

Re: Manual modification of thickness and nodal eccentricity to simulate wear

Phenom
Phenom

Hi RMS,

 

first of all I use NX10 and I guess there is no way to define a spatial distributed offset in NX10, but It's only an assumption. I believe you have a newer version. So maybe there are more capabilities which I don't know.

 

Besides, in your formula for offset is a spelling error. "thikness" instead of "thickness".

 

When I 've used "thickness/2" as expression I've got the error  "constant expression cannot contain variables..." see picture below.

And as I did change the formula to a real user defined constant expression "OFFSET_VALUE/2" with OFFSET_Value = 0.1 mm then it works.

 

In my case "thickness" provides a value of 1 mm and this is the default value of my PSHELL-property. So "thickness" looks like "Default Thickness". I don't know the expression for using the distributed thickness provided by Table field. But in the dialog "Function" I've found "THICK() - local thickness at the input point". But I didn't understand the functionallity as I should have name the input point. I don't know what it means.

 

My table field is as following.

SHELL_THICKNESS_REDUCTION_TableField_001.png

 

SHELL_THICKNESS_REDUCTION_TableField_003.png

 

 So therefore, I'm out here. Maybe someone other can help you with better information.

Best wishes, Michael

| Production: NX10; Development: VB, TCL/TK, FORTRAN; Testing: NX12 | engelke engineering art GmbH, Germany | 2019-07-08
| Kudos for good posts! And if my post answers your question, please mark it as an "Accepted Solution". Kick Off (2015-09-14)On the Map (2016-10-21)1st Gear 2018 (2018-02-19)5th Birthday! (2018-02-25)Popular (100, ‎2018-10-30)Prolific (100, 2019-02-27)Philosopher (500, ‎2019-02-28)Problem Solver (50, 2019-06-25)

Re: Manual modification of thickness and nodal eccentricity to simulate wear

Solution Partner Experimenter Solution Partner Experimenter
Solution Partner Experimenter

Thanks Midi1791 for your time.

When I'll find the answer I w'll  share with you.

 

By the way, do you know how to export and import a manual mesh using a.dat/.txt file
with individual sentences like these???:

grid i 11 x 1.2 y 25.0 z 10

grid i 12 x 2.0 y 25.0 x 10

grid i 13 x 2.0 y 30.0 x 10

grid i 14 x 1.2 y 30.0 x 10

...

..

etc.

 

element cshell4 i 1 grid 11 12 13 14 material 2 thickness 6.5 eccentricity -2.0

...

etc.

 

Maybe, if I import something like this and after to apply the remaining BCs and loads. In this case I don't need associativity between cad and fem models. The idea is to reuse a existent fem model to update a structural calculation to asses mechanical integrity under wear.

Re: Manual modification of thickness and nodal eccentricity to simulate wear

Phenom
Phenom

Hi RMS,

 

you can import existing NASTRAN decks as *.dat structures into an existing FEM with File => Append.

 

But you have to respect the syntax of nastran deck. Maybe try the following:

 

- Write your model as NASTRAN deck into dat file,

- Identify element block and import it (CQUAD8 and CTRIA6) into Excel

$*
$*  NX Mesh Collector: THICKNESS_1mm
$*  NX Mesh: 2d_mapped_mesh(1)
$QUAD8       EID     PID      G1      G2      G3      G4      G5      G6
CQUAD8         1       1       1      40      41       2    1522    1523+
$             G7      G8      T1      T2      T3      T4   THETA   ZOFFS
+           1524    15251.8500021.8500021.6999991.850002             .05+
$          TFLAG
+              0
CQUAD8         2       1       2      41      42       3    1524    1526+
+           1527    15281.8500021.6999991.6999991.850002             .05+
+              0
CQUAD8         3       1       3      42      43       4    1527    1529+
+           1530    15311.8500021.6999991.6999991.850002             .05+
+              0
...

- See that a bulk data entry of CQUAD has three lines and in second line the last value is Offset.

T1 - T4 are the element thickness at corner nodes G1 - G4.

- Try to calculate offset by means of average of reduced thickness in excel.

- Export it as ASCII again and substitue old element block with the new one and reread dat file in NX. (It depends on your license if you can do it.)

 

Keep in mind: CTRIA elements have another structure of bulk data entry.

 

Second way:

Or you can append the element block alone into an existing FEM without elements. Therefore delete all elements in your FEM without deleting nodes (keep Orphan Nodes) and append your modified elements. A existing Sim should not be affected, if in the first place the sim was build by using an appended fem without geometry.

 

Info: Every value or keyword in a bulk data  entry is 8 digits long and one line consists of 10 values or keywords. "+" at the beginning of 10th or 1st word means continuation in next line or from previous line.

 

Maybe it works. Best wishes, Michael

 

| Production: NX10; Development: VB, TCL/TK, FORTRAN; Testing: NX12 | engelke engineering art GmbH, Germany | 2019-07-08
| Kudos for good posts! And if my post answers your question, please mark it as an "Accepted Solution". Kick Off (2015-09-14)On the Map (2016-10-21)1st Gear 2018 (2018-02-19)5th Birthday! (2018-02-25)Popular (100, ‎2018-10-30)Prolific (100, 2019-02-27)Philosopher (500, ‎2019-02-28)Problem Solver (50, 2019-06-25)