Abaqus frictional generated heat model 1

[sztatty]

Hello

Found out that I posted this thread in a wrong forum group, hope this is the right place.

So, in Abaqus I managed to create two objects with contacting surfaces, pressed to each other while one is fixed and the other is moving with a constant velocity. The simulation seams fine for stress results, but at temperature it shows no change at all. I tried different BCs and predefined fields for temperatures and some other adjustments, but no goal. What could be wrong? Attached my cae file. Would appreciate some help.

 

[burningDiesel]

I'm using abq 6.12, so maybe something went wrong in converting.
But here is your problem:

You are doing static stress displacement analysis, so you are getting the stresses and displacements.
If you want to get a temperature, use the coupled temperature displacement step.
Also, use the C3D8T elements to free up the thermal DOF.
Changing this, I got a very small temperature result using your values (2.5e-4). If this is not what you expect, check to make sure your units are consistent.

 

[sztatty]

Thank you for your reply! Your suggestions sounds valuable and I will test them home toight. Also I did not thought that there were any temperature change, just looked on the result animation and saw plain constant blue.

 

[sztatty]

Made the changes as you advised and the temperature results were really that small (but at least there was a real change in temperature), so I revised and adjusted my units and now they are all in SI but the results remain.
Only one thing is not really clear for me with the units and that might needed to be fixed. This problem is related with the model. Like if all units are in SI then are the part's sketch dimensions also in SI (m)? So if there is a r10 radius in the sketch it means that it is 10 m, so in that case I should resize it to r0.001 to have 10 mm radius? (guess that will make a huge change in results since the load would be very small in that first case, but had no time to try this out jet)

Further that the BCs velocity behaves strange. If I change V1 from 1 to 2 I expect twice the distance gaind by the moving part (while the step's time period remained the same), but insted what I expected the moving part moved to the same place, apparently with the same speed. The strangest behavior accured with much higher velocity. The moving part went to the same place with the same visible velocity, but the temperature change in the fixed plane ovetook the moving part far ahead which is absurd. So Is there a distance and velocity limit for the displayed part motions in the results, or what could be wrong?

 

[burningDiesel]

I rechecked your .cae file. You should put NLGEOM (non linearity) on. Large displacements & contact should do it.
Furthermore, you should constrain your cylinder in the Y direction, to avoid numerical singularities. The reason your simulation still runs is probably because of the frictional contact, still, you should properly constrain everything.
If you use SI units, indeed dimensions are in meters. so 10 is 10 meter.

 

[sztatty]

Will check that too. Thank you again!

 

[sztatty]

So tried the suggestions a while ago and rescieved encouraging results, but had no time but now to write about it. The most problematic part for me was the proper setting of the time increment. (What worked out for me was: time period 1; incrementation type: automatic; max. number of increments: 1000; increment size: initial 1E-009, minimum: 1E-009, maximum: 1)

 

[IceBreakerSours]

I noticed some flags in the posters' comments here and felt compelled to make a few comments.

..the other is moving with a constant velocity

Velocity has NO meaning in a static analysis!

..just looked on the result animation and saw plain constant blue.

This is perhaps one of the reddest flags. I strongly recommend not to focus on colors and animations AT ALL before you have looked at the numbers. This is no rule and there are exceptions but, if you are a beginner, then take this as a rule.

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[sztatty]

"- *Please, please, please do your homework before you post*." I'm polite, but thank you.

 

[sztatty]

Othrvise, I don't see your point, feel free to explan, but consider: (use google if not unequivocal)

7. This forum reaches out to engineering professionals worldwide, many of whom are not native English speaking. When responding to non-native English posters, please refrain from disparaging their use of English; ask for clarification where necessary.

 

[IceBreakerSours]

sztatty:

Feel free to correct me; I may simply have misunderstood what you wrote. Indeed, I'd like to know where I went wrong in my (mis?)interpretation.

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[IceBreakerSours]

My comments had nothing to do with English and everything to do with the implication of the engineering terminology used. Native and non-native English speakers make those mistakes.

Static analysis, as the term implies, is carried out for a point in time. So, one is not concerned with how, for example, the stresses evolve over a period of time. Time, in FEA, for static analyses is simply a numerical parameter that allows the numerical procedure to apply a portion of external load and try to establish equilibrium, if 'possible'. Therefore, speed/velocity (delta_s/delta_t) is, by definition, irrelevant in a static analysis because delta_t is not the "time" you expect. The time you expect shows up in quasi-static, dynamic or explicit analyses.

Next, colors in an FE analysis are simply mappings of results. In a static stress-displacement analysis, for example, color may stand for some stress (von Mises, I guess, is the default stress in Abaqus/Viewer) or contact pressure or a field variable etc. But color scales are simply for visualization of the underlying results. Say, the computed stress in a region varies from 1 MPa to 20 MPa. ABAQUS post-processor uses this information to create a scale of colors (typically, from blue to red in 10 units). [There is also averaging at nodes, and scaling to be kept in mind.] If one is not aware of the results at nodes, elements, interfaces etc. and the discontinuities, looking at colors, in all probability, is simply a disaster waiting to happen. What one must be aware of is, for example, reaction forces at nodes of interest, rather than a plot of von Mises stress. Why? That's where the theory of FEA and structural mechanics comes in to play.

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[sztatty]

I was not looking for stress results. My main problem/task was related with heat flux and obtained temperatures in transient case. Literally my goal was to visualise temperature differences in macro sizes confirming my expectations which was achieved with the help of the first commenter. (Used ploted results for specific node elements for comperson of calculated results and gaind success, but this was not related to this topic. I had much more novice problems with specific settings.) And I see your point about what you mean with how I evaulated results, will keep in mind, but when the legend and the colors show no change, that means something too.

 

[IceBreakerSours]

Overall, my comments are meaningful whether stress or temperature or any other field variable is of interest to you.

As sdebock pointed out to you, using the appropriate analysis, elements, constraints etc. will let you carry out a thermomechanical analysis in the right way. However, my comments had to do with implicit issues.

For example, in the step definition, note that the type of analysis is Static, General. In the description, you wrote Apply velocity and "time period" is 10. In the load definition, you are applying a load of 0.2 units on top of a surface. Now, what you are really doing is applying 1 unit of pressure (10 x 0.1 = 1.0) on top of the surface at "time" = 10. [Here, as pointed out in my previous post, time has no meaning except as computational parameter.] If that is what you wanted to accomplish, great! If not, then I am sure you'd agree that you ended up correctly solving the wrong problem. Why wrong problem? Well, because you may really have wanted to apply 0.1 units of pressure on that surface at a particular speed in a given direction. In that case, the Implicit Dynamic analysis may be more appropriate.

.. when the legend and the colors show no change, that means something too.

If you expect a wide variation, in say temperature, in a given region and you do not see any variation in colors, then yes, you are correct. But, I guess, if there is little to no variation, then there should be little to no change in colors too. Besides, it also depends on how many colors (levels) are chosen. In ABAQUS/Viewer, you can go up to 20 levels, if I remember correctly. Note, however, that there are situations where even this may not necessarily be true but those situations arise in advanced features in FEA.

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[sztatty]

If I'll have time and need to continue with this task which is probable, I'll check implicit dynamic analysis too, but as sdebock pointed out for me the coupled temperature displacement analysis worked decently. And yes I was looking for a wide variation in temperature. Practically I had the opportunity to vary my inputs to get results similar to something observed that could have been confirmed with calculations too. My unfortunate and unprofessional statement with the colors ment only that there was something not going well in my simulation as I expected.

 

[Kamuro]

Hi,

did you successfully finished your simulation? I'm also doing something similar and I just wondered if you could post your final .cae file. Would be very grateful for that. Thanks!