Hello Everyone !
I'm doing analysis of a welding process using Coupled Eulerian-Lagrangian approach in ABAQUS/explicit. I have created a model (two layers of workpiece, one eulerian part, and a rigid tool). The tool penetrates the two layers of workpiece (one above the other) and is under pressure till the end. The feed rate given is 50 mm/sec and angular velocity 400 radians/sec. High feed rate is used to complete the analysis quickly. A predefined temperature of 293 K is specified for the entire model and a total step time of 0.08 sec. General contact (all with self) is specified in the interaction with coefficient of friction=0.4. The eulerian part was specified workpiece material by creating discrete fields using volume fraction tool and then using material assignment tool in the predefined section of loads module. The eulerian part is specified with a zero displacement/rotation boundary condition in all directions. In the analysis results till 0.03 seconds, the tool is penetrating the wokrpiece but the temperature profile isn't physically meaningful. the maximum temperature at 0.0456 sec is just 320 K, while the temperature on the tool is way too high, about 1850 K
Can someone point or suggest where I may have gone wrong in the creation of model ? Also, I've noticed that at the boundary regions between void and discrete field, the temperature is dropping below 293 K and at some places it's even going to zero. I'm attaching image of temperature distribution in the workpiece and also the model created
Thanks.
Subscribe to and seek assistance from the
ABAQUS mailing list
https://groups.yahoo.com/group/ABAQUS
Search the archive before posting.
Good luck
Frank
Recheck the assigned material model for the rigid body(if you tell me what is the rigid body material model I might be able to help you more)
And assess the defined temperature units consistency between each material model and the absolute zero temperature of the whole model defined at attributes
Ardalan,
Hello.
I'm using 316 L steel (solid, homogenous section) for the tool body for which conductivity, specific heat, yield strength, are specified in the material property section. I've used Kelvin throughout the model and absolute zero is 0 K .
Thanks
OK
What about the heat transfer parameters of the modeled tool cooling mechanism (i.e. the heat exchange between the tool and the surrounding environment due to be defined at Interaction Module)
and tell me what is your expectation of tool max. temperature according to the real world practice. I am asking this regarding the annealing possibility of your tool.
As Ardalan mentioned you need to check the heat transfer parameters of the modeled tool cooling mechanism (i.e. the heat exchange between the tool and the surrounding environment due to be defined at Interaction Module) at first.
Dear All,
I've specified zero surface convection and radiation properties on the side surfaces of the workpiece, and the temperature profile has improved a bit. As far as interaction module is considered, I've specified 0.4 as co-eff. of friction, normal behavior with hard contact and no separation, 100% of friction is converted into heat and 71% is transferred into the workpiece and pressure based gap conductance has been specified.
Regarding the maximum temperature, 80-85% of the melting point of the tool material is expected to be reached (1200-1300 oC).
Hope that answers questions of Ardalan and Roozbeh.
Thanks.
Why you nullified convection and radiation ? Does that decision has anything to do with the reality ?
And something else that I forgot to mention at first, why you defined yielding strength and the corresponding plastic strain for your rigid body ? (a rigid body is going to ignore the deformation due to any stress) and maybe that is exactly why its temperature is unrealistically high. i.e. letting the component deform in reaction to the stress induced by friction heat makes it use the heat in two real world ways 1.Expanding 2.Heat exchange with environment
You have not modeled non of the above so you get that wrong temperature for your tool.
Here is my suggestion after all:
Firstly define relevant heat transfer mechanisms with non-zero real values, if it again fails to satisfy the reality then go ahead and make your tool a deformable body with all the defined parameters of yours for the tool plus the expansion coeff. to let the tool material to model the thermo-mechanical interaction and subsequently lead the tool to use the friction heat as real as possible.
Last but not least, regarding your predicted temperature range, you gotta define annealing temperature for your tool otherwise you will get wrong stress magnitude for your tool (kinda same story as the temperature)
Dear Ankit,
I am doing a CEL model for Friction stir Welding, and I believe your issue is for two reasons:
1- Check the work piece density, make sure it is not very large due to unit inconsistency or maybe you are doing mass scaling in a wrong way.
2- Step time is very small which will not allow the temperature to rise, unless you are also decreasing, with the same factor, the specific heat (time scaling).
I hope that helps you.
Regards,
Mohamed
Hello Mohamed Badreldin,
I did resolve the issue of abnormal temperature by verifying the material properties and loads. I have another question for you, what workpiece material are you using and how are you performing time scaling?
Hello Ankit,
I am using AL 6061-T6 for the workpiece. Now Iam using mass scaling in my model, but you can use time scaling by reducing both step time and specific heat with a constant factor. You can refer to attached study showing comparison between mass scaling and time scaling in CEL.
I hope that answers your question.
Regards,
Mohamed
- Badges
- Science topic