Coupled temp-disp analysis

[MNS747]

hi
I have got few questions
first off all I am doing coupled thermal displacement analysis on a machine tool spindle with two sets of bearings as generators of heat. I made a simple heat transfer step and have seen the thermal gradient in 600s (10min) that means it was working fine. Then I tried to see displacements due to the thermal gradient. I copied the model and replaced it with coupled temp-disp analysis. Included mechanical properties for eg youngs modulus, poisons ratio, coefficient of thermal expansion. Made the transient step equally to the heat transfer time. I mentioned interactions as surface to surface etc. Entered a predefined field as "reading from previous session" and entered thermal.odb with step 1 and increment 1 (thats what i assume it will start reading temperatures from 1st increment of 1st step of heat transfer analysis).
Now what it does, the thermal gradient which I saw in heat transfer analysis at 600s (10min), that is being shown in only 10s in coupled analysis. and showing me funny shapes of displacement which dont have any connections to the reality. I have tried the same by generating heat and monitoring displacements in only one coupled temp-disp analysis instead of reading results but still doing the same. what am i doing wrong. I hope I am clear to some extent and able to clarify the problem.

Any answers to this will be highly appreciated.

 

[corus]

I don't think you are doing a coupled temperature-displacement model as this runs both the thermal and stress analysis at the same time. It seems you're running a thermal analysis first and then reading the temperatures in from a separate thermal analysis. '
One problem I have seen in the past is that the stress model doesnt have the same node numbering as the thermal model. The temperatures that are loaded are then apparently dispersed randomly around the model, depending on the new node numbering. This leads to some odd results. If you can use the thermal model you created and simply change the element type to a stress type element in the mesh module of CAE. I think there's also an interploation option for applying the temperatures to nodes that may not match.
You'll have to modify the loads and applied displacements and the step from heat transfer to static stress making sure you have the same time steps as the original thermal analysis. Also make sure you have loaded the temperatures correctly by including the temperature as an output variable. It's either NT11 or NT, you'd have to check that in the manual.

corus

 

[MNS747]

hi corus
Thank you very much for your advice.
Yes I am reading the temperautures from an existing thermal model. After reading your post i feel that you are suggesting to replace the coupled-temperature displacement Step with Static general Step. am I right?
One thing i am not sure is after selecting "reading from previous session" in predefined field, I am entering Step1 increment 1, does it mean Abaqus should start reading provious thermal odb from step 1 and increment 1?

I had a mesh problem and I have used virtual topology in it and unsure if it is affecting the temperature distribution.

Regards

 

[corus]

If you're reading transient temperatures and want to see the effect this has on stresses over the same time then you will begin from step 1, inc=1 and end at step n, inc=m. I tend to use the same total time interval and time step as the thermal analysis to make it neater but I don't think it's necessary in all cases. You can of course simply read in the temperatures from a set time and apply these as thermal loads to your model. This can lead to problems though as you'll be introducing a sudden change in temperature and the time step might reduce significantly to ramp the temperatures up gradually. It may also affect the solution if you have plasticity and thermal cycling involved.
Without looking at the manuals I'm certain that there's an incompatible mesh option you can check that will transpose and interpolate/extrapolate the temperatures to the geometry of your model even if the node numbering isn't the same. As I said before, it's wise to check that the temperature distribution you are applying is the same as that obtained from your thermal model so have temperatures as an output variable, along with your stresses/displacements etc.

corus