Verifying Mecway Results to Ansys Mechanical

CainiteCainite
Hey

I'm current trying to decide on buying Mecway.

So far I like the intuitive GUI but before I'm going to buy it I want to verify it against ANSYS Mechanical Application test cases https://ansyshelp.ansys.com/public/account/secured?returnurl=/////Views/Secured/corp/v252/en/wb_vm/wbvt-vm-mech-wb.html.

I'm trying to complete VM-WB-MECH-002

Materials
E=1000 Pa
v=0

FEM
745 Nodes
2601 Elements (Tet4)
8940 DoF
Mesh Size ~1.5m
Mesh Bias ~0.075m Along Hole Edge

Boundry Conditions
Constraints: fixed on side face surface


Software
Pre/post: Mecway
Solver: Internal

Load Case 1
-Opposite face: Pressure of "-100 Pa" in the x direction

Results
Target - Maximum Normal Stress (Pa)-312.5
Mecway - Maximum Normal Stress (Pa)-277 (Element), 250.9(Node)
Error - 12.8%

Synthesis of Results
Due to the limitation of the free version of 1000 Nodes, I have not reached convergence yet.

I am still quite a novice at FEA (only 1-week in), so I may have gotten somethings wrong. I have experienced workmates which is why I'm presenting in this way.

Can someone with a paid version try to verify this test case for me??

Much Appreciated
Cainite

Comments

  • CainiteCainite
    Results
  • CainiteCainite
    I'm sorry I think I calculated No of DoF incorrectly. 745 Nodes * 3(Tet4) = 2235 DoF
  • cwharpecwharpe
    edited August 2025
    Answers will vary a bit with element selection. Definitely better with higher order (Quads vs Linear). A quick model using 2nd order shells and Symmetry. The Test said something about just two refinements. Attached are my results using hex20's extruded from Quad8's.

    Highly recommend the purchase. At the basic level, the GUI is so-o-o-o-o much easier than others I've used.

    P.S. Incidentally, per Test, your hole radius = 0.5 m, no?



  • CainiteCainite
    That awesome! I have alot to learn.

    Good pickup on the I skimmed over and thought it said 0.5m diameter not radius

    I'm getting 305.5 Pa, Error 2.3%. Now using Tet10.

    How did you create such a clean mesh? Did you manually mesh it?

    I am starting from Alibre Atom3D part file and creating a idealized version by spliting it in half. I can't find a way to specify hex8 or hex 20 mesh autogen it always force me to use tet10.

  • CainiteCainite

  • CainiteCainite
    Ok got it! 316 Pa Thanks! Now for the next tests
    3.JPG 82.3K
  • cwharpecwharpe
    Yes, I did mesh by hand. Simple Rectangle Shell/ Refine evenly to locate center for Hole Tool.

    Your Test was asking for Max Normal stress (tension in the direction of the load). I see you reported the von Mises stress. Maybe see what you get from the Principal Stress output? Yes, they are close in this case but vM is scalar, derived from up to (9) stress components, and has no directional reference. ;)
  • FatmacFatmac
    I got pretty close with some finer meshes -with more refinement and hex 20 blocks i got a max VM of about 318 MPa. I found all the test in one doc at https://ansyshelp.ansys.com/public/account/secured?returnurl=/////Views/Secured/corp/v252/en/wb_vm/wb_vm.html. I had a quick go at the buckling of a step column example and got a pretty close answer for that one also
  • SergioSergio
    Hi @Fatmac , did you see the cases 4 and 6? I did others cases and agree very well
  • FatmacFatmac
    Good evening Sergio -i've had a play with a few examples but 4 and 6 are a little out of my capabilities - i will take a look when i have more time
  • disladisla
    @Sergio

    Me I was also finding some discrepancy too.
    I have look at the source of that problem and solve the equation again.
    Arpaci, V. S. (1966). Conduction Heat Transfer. Addison-Wesley Book Series. (p. 130).
    Free acces:
    https://archive.org/details/conductionheattr0000arpa_k8i6/page/n3/mode/2up

    Solution is T=482 ºF not 476 ºF




    *MATERIAL,NAME=MATERIAL *DENSITY 1000 *CONDUCTIVITY,TYPE=ISO 555.1,0 563,4.3 662.4,58 761.9,111.8 861.3,165.6 960.8,219.4 1060.2,273.2 1159.7,326.9 1245.2,373.2 1259.1,380.7 1358.6,434.5 1458,488.3 1557.5,542 1656.9,595.8 1756.4,649.6 1855.8,703.4 1955.3,757.2 2054.7,810.9 *SPECIFIC HEAT 100,0 100,4.3 100,58 100,111.8 100,165.6 100,219.4 100,273.2 100,326.9 100,373.2 100,380.7 100,434.5 100,488.3 100,542 100,595.8 100,649.6 100,703.4 100,757.2 100,810.9 *SOLID SECTION,ELSET=MAIN,MATERIAL=MATERIAL *INITIAL CONDITIONS,TYPE=TEMPERATURE TEMPERATURE_NODES(2),373.15 TEMPERATURE_FACES(2),373.15 *PHYSICAL CONSTANTS,ABSOLUTE ZERO=0.,STEFAN BOLTZMANN=5.669E-8

    Regards
Sign In or Register to comment.

Howdy, Stranger!

It looks like you're new here. If you want to get involved, click one of these buttons!

Sign In Register