Tek-Tips is the largest IT community on the Internet today!
Members share and learn making Tek-Tips Forums the best source of peer-reviewed technical information on the Internet!
-
Congratulations TugboatEng on being selected by the Eng-Tips community for having the most helpful posts in the forums last week. Way to Go!
Comparing Hex, Tetra and Beam mesh
- Thread starter sylwcios
- Start date
- Thread starter
- #2
So one more time,
The problem is,
I have done some simple calculation as shown on the pictures.
I used different mesh sizes and types, so I have different results.
Using solid elements the results are the same in terms of displacement, there is small difference in terms of stresses.
However using beam elements the results differ a lot. Stresses are almost halved as well as displacements.
Why is like that and what is closer to the true?
thanky you guys
The problem is,
I have done some simple calculation as shown on the pictures.
I used different mesh sizes and types, so I have different results.
Using solid elements the results are the same in terms of displacement, there is small difference in terms of stresses.
However using beam elements the results differ a lot. Stresses are almost halved as well as displacements.
Why is like that and what is closer to the true?
thanky you guys
Hi,
To understand which model gives the closest value to the "reality" you should know this "reality".
To do so you have to do a theoretical calculation of this simple cantilever example.
Then compare the results (deflection, stress...) with each value you obtained from the shown models.
I would say that the Hex fine mesh will be the closest one to the analytic results.
for the beam elements stress do not forget to take the maximum absolute value between End A Max / Min and End B Max / Min.
Regards,
Seif Eddine Naffoussi, Stress Engineer
33650 Martillac – France
To understand which model gives the closest value to the "reality" you should know this "reality".
To do so you have to do a theoretical calculation of this simple cantilever example.
Then compare the results (deflection, stress...) with each value you obtained from the shown models.
I would say that the Hex fine mesh will be the closest one to the analytic results.
for the beam elements stress do not forget to take the maximum absolute value between End A Max / Min and End B Max / Min.
Regards,
Seif Eddine Naffoussi, Stress Engineer
33650 Martillac – France
one "obvious" thing is that your "beam" model looks like a bunch of surface plates, whereas the othe rmodels are solid shafts.
not all elements are created equal. for example TET4s are very stiff elements, and TET10s are preferred.
i wouldn't expect too much difference between TETs, HEXs, other solid elements. the plate model is clearly quite different, and plate elements don't particularly like varying stress (like from the NA up to the peak bend stress). try using a linear beam element to model the shaft.
as posted above, for simple models you can figure out the real result and so verify the model.
another day in paradise, or is paradise one day closer ?
not all elements are created equal. for example TET4s are very stiff elements, and TET10s are preferred.
i wouldn't expect too much difference between TETs, HEXs, other solid elements. the plate model is clearly quite different, and plate elements don't particularly like varying stress (like from the NA up to the peak bend stress). try using a linear beam element to model the shaft.
as posted above, for simple models you can figure out the real result and so verify the model.
another day in paradise, or is paradise one day closer ?
- Thread starter
- #5
"one "obvious" thing is that your "beam" model looks like a bunch of surface plates, whereas the othe rmodels are solid shafts".
The obvious thing for you is a 'thickness,corss section' option in Femap which is switch on only for visualization purporse, shaft is made of linear beam elements.!!
Hand calculation I have done is: F*l/Wx= (100*15,5)/21,2=73,09 MPa. So the value is equal to the one from the beam analysis. Even if I influence a shear force I won't get the value from other solid anaylis and for this reason I am bit confused.
What do you think guys?
The obvious thing for you is a 'thickness,corss section' option in Femap which is switch on only for visualization purporse, shaft is made of linear beam elements.!!
Hand calculation I have done is: F*l/Wx= (100*15,5)/21,2=73,09 MPa. So the value is equal to the one from the beam analysis. Even if I influence a shear force I won't get the value from other solid anaylis and for this reason I am bit confused.
What do you think guys?
ok, i missed the line elements on the axis. i'd change visualisation to "show shape"
i don't know what "combined stress" is, but the picture is very odd of a beam in bending.
i think your hex model is probably closer to the right answer, the stress spike is due to the constraint; if you look a little down the shaft from the end, the number look about right. i think your beam model may be given the "right" answer because the element stresses are not responding to the constraint.
try a pin ended SS beam.
another day in paradise, or is paradise one day closer ?
i don't know what "combined stress" is, but the picture is very odd of a beam in bending.
i think your hex model is probably closer to the right answer, the stress spike is due to the constraint; if you look a little down the shaft from the end, the number look about right. i think your beam model may be given the "right" answer because the element stresses are not responding to the constraint.
try a pin ended SS beam.
another day in paradise, or is paradise one day closer ?
- Thread starter
- #7
Thank you for your answer! indeed just below the stress spike in solid analysis the stresses are very similar to those from the beam analysis.
Is there any option to avoid the stress spike occurence in solid element analysis?
I can't find "show shape" visualisation option can you tell how I can find it?
Is there any option to avoid the stress spike occurence in solid element analysis?
I can't find "show shape" visualisation option can you tell how I can find it?
"show shape" is under view/options ... one of the element options.
i think the probelm with your constraint is that it looks to be fully fixed. a "better", more real world, constraint might be to use radially oriented springs; allowing the nodes to move ever so slightly (as opposed to a rigid constraint "thou shall not move").
part of the real world, that the FE is detected, is that as the shaft bends it'll contract along the vertical diameter, and expand in the horizontal. This affects how the shaft responds to the hole it's sitting in.
another day in paradise, or is paradise one day closer ?
i think the probelm with your constraint is that it looks to be fully fixed. a "better", more real world, constraint might be to use radially oriented springs; allowing the nodes to move ever so slightly (as opposed to a rigid constraint "thou shall not move").
part of the real world, that the FE is detected, is that as the shaft bends it'll contract along the vertical diameter, and expand in the horizontal. This affects how the shaft responds to the hole it's sitting in.
another day in paradise, or is paradise one day closer ?
- Status
Similar threads
