I'm a beginner in FEMAP and i want to know how i can move ("walk") a heat source on a plate. I want to simulate the welding process and i want to know the stress and deformation on the plate for diferent temperatures.
Let's say i have this plate of 1000x1000x8 mm. And i want to "walk" a heat source of 500 celsius degress from point A to point B and then see the VonMises stress and total translation. (If the source is 500 celcius degress the results of the vonmises stress will be in N/mm^2? and Total Translation in "mm" )
Can somebody tell me how to do that?
It's quite a question, but in short, you need a transient heat transfer analysis (to get the temperature results) , followed by a multi-step non-linear static analysis (where the multiple steps of temperature results become multiple temperature loads in the mech analysis) .
You will have to create several time functions which ramp up and ramp down the temp according to the profile (duration AND location) you want. Each node will then need its relevant time history function of temperature profile called up for the temp load applied. There is no "walk the load" button as you might hope.
But, temperature load is like a "constraint" - if you apply a temperature history rather than a flux profile or a convection, then the temperature is explicit (absolutely as specified) at its applied location, rather than a by-product of the heat input - you may be better to apply a convection with a "very high" coefficient, convecting to the desired temperature. And note the convection coefficient can also have a time function applied if you want to (eg). ramp up the temperature quite explicitly, but cool by environment rather than by control.
For transient heat transfer, you must include both conductivity and specific heat in the material properties.
You allude to units. I suggest you google: Femap consistent units and refer to the Endurasim pdf.
Once you have succeeding in doing the transient heat transfer, you will have temperature output from multiple time steps.
Output Sets of temp results should then be a load case in the multi-step non-linear analysis. Model -> Load -> From Output can be used to create temperature loads from temperature results... one Load Set from each Output Set that produces useful results at an appropriate interval in time.
You need one extra load set which is used as the initial temperature condition - with the starting temperature applied to the nodes for that initial condition load set.
You need to make sure you have an expansion coefficient for the material, otherwise no thermal deflection will occur.
You need to make sure you have some form of mechanical constraint applied in the multi-step nonlinear analysis, otherwise the analysis will fail or struggle due to singularity. And also note that thermal strain can occur without thermal stress unless some part of the "structure" and/or some external constraint is resisting the thermal strain.
This is a very brief outline of the basic steps - if you are a beginner with Femap, it's probably not the easiest first project to be working on!