You time curve should be:
At time 0 we have 0 load at time 1 we have a load factor of 1
You BC should be the temp you want to raise the item to so 1 times the temp equal the target temp.
If we the thing expands (I assume it will expand) will it them buckle? In other words are you trying to figure out if the thing will buckle do the linear expansion to due a change in temp? If so you need more info to pull this off. Happy to fill you in if you tell us the process you are applying to get where ever it is you want to go (please state that as well).
Thanks for the response Bill.
I am attempting to use the temperature loads to cause an initial stress prior to the column being loaded in axial compression. That's why I want to have the temperature be 0,1 and 1,1 (constant throughout the study) and the axial load will be 0,0 and 1,1 (0 and time 0 and 1 at time 1).
This method works when applying a small initial lateral force to induce buckling (I use 0,1 and 1,1), but I am still not convinced as to why I cannot use it with a thermal load.
To avoid confusion, I'm using 500 as my end time so I can easily tell when column fails when applying a 500kN force (hence the 500 in my screenshot).
To address your last comment - the expansion due to the thermal loads will not cause buckling, rather they will decrease the buckling load because the cross section is already stressed. I am going to use the thermal loads to try and simulate residual stress caused by the manufacturing process of W-Sections. The attached model is very simple indeed - I'm just trying to do some calibration with a basic Euler case before moving to more complex cases.
Hopefully the above provides some clarity.
As a side note:
Even if I do define the load application in the manner you suggest (which seems to be the default application that solidworks uses if you do not check the time curve option), I get the same problem. This is why I initially thought it was a SW bug.
I think I get what you are trying to do now. You want to get a beam (or whatever) and you want tog et it to a state of stress that approximates some manufacturing operation input. Then you want to get an estimate of the buckling strength. If it was me, I would do a three step analysis:
1) step 1: apply forces to get the initial stress distribution you want - they should sum to zero but provide a stress distribution in the model.
2) step 2: apply a small transverse force sot he thing isn't "numerically perfect"
3) Step 3: apply and axial load till the analysis fails. The last competed load step will be a number that is slightly less than the buckling load.
time curve will look like
for step 1 forces
Force step 2 force
3,1 (could easily be 0 - doesn't much matter)
For Step 3 force (bigger than you think it will support but not super huge)
Some excellent advice there - thanks very much Bill. That seems to do the trick!
I do have one followup question though:
Previously I was choosing a number of steps that corrisponded with the applied load (ie 200 steps for 200kN). Then I could easily identify when failure occured (150s = 150kN). Now that I'm only using 3 steps - is there an easy way to display failure load in SW, or do I just need to use simple fractions to figure out where my model failed?
time=load in a NL static analysis. Hitting 50% of the load would occur at a time of 0.5 sec. in a force controller solution. So the in the case above a time of 2 sec = zero on the buckling load, at time of 2.5 sec would 50% of the applied buckling load.
Great - kind of a silly question now that I think about it but thanks for the clarification none-the-less Bill.