March 8, 2021 at 2:56 pmmichutorresSubscriber
My work consists on a adhesive melting simulation in a deposit. The adhesive should start solid and becoming fluid as it gets warmer because a heat flux inside the deposit of aluminium.
When a run calculation in Fluent, I am getting an error that says 'Floating point exception'. I am going to explain all the set up.March 8, 2021 at 3:33 pmYasserSelimaSubscriberTime step size is too large. make it 0.001 ... and maximum number of iterations, at least 20nMarch 8, 2021 at 4:12 pmmichutorresSubscriberOk I will try this.nIn reality, adhesive takes 30 minutes to get totatlly melted, so that means 1800 seconds. If I put 0.001 time step size, I would need 1.800.000 Number of steps. That would be ok?nMarch 8, 2021 at 4:17 pmYasserSelimaSubscriberTry to get convergence first, then use adaptive time step and let fluent decide the optimum sizenMarch 8, 2021 at 4:19 pmmichutorresSubscriberWhat do you mean with 'try to get convergence first'? How can I ckeck this?nMarch 8, 2021 at 4:24 pmYasserSelimaSubscriberI mean make sure solution do converge first. Try few time steps ... make sure the residuals decrease every time step until they reach constant value or go below the set criteria. nThen think how to optimise the solutionnMarch 8, 2021 at 4:42 pmmichutorresSubscriberSolution didn't converge. Can you please recommend me which models I should enable for my case? I enabled Energy and Solidifcation & Melting.nWhat about viscous (laminar)?nI am not understanding why it doesn't converge.nMarch 8, 2021 at 4:49 pmYasserSelimaSubscriberIf you have laminar flow, use laminar.nMake the density as a function of temperature for your material. this is important to model natural convection in a liquid.nMarch 8, 2021 at 4:57 pmmichutorresSubscriberOk I will change the viscous model from k-epsilon to laminar.nFor the density definition I used Piecewise-linear and I introduced 2 points depending the temperature (K) (910 kg/m3 at 313 K and 790 kg/m3 at 398 K).nI don't have any natural convection. All faces are adiabatic. The only one boundary condition that I have in my model is a heat flux in a wall inside the deposit.nWhat do you think?nMarch 8, 2021 at 7:09 pmYasserSelimaSubscriberFor any fluid, if the density changes with the temperature and there is a room for circulation, natural convection will occur nMarch 8, 2021 at 8:32 pmmichutorresSubscriberYes I know. I thought you were talking about a convection between the air and the adhesive. nDo I have to insert the convection coefficient h of the contact adhesive-deposit? Or is the program who calculates it once the adhesive starts to get melted? nMarch 8, 2021 at 10:01 pmYasserSelimaSubscriberno you don't have to, but you need to insert the thermal properties in the material panelnMarch 9, 2021 at 8:24 ammichutorresSubscriberok thank you.nI got the density as a function of temperature: Density=3'9286 T^2-57'929 T +984nDo I have to create a Named Expression or UDF? Or can I write this formula directly in the material properties panel selecting piecewise linear or polynomial or bussineseq? nMarch 9, 2021 at 9:10 amYasserSelimaSubscriberIn the material panel , polynomial ... Bussineseq will not work in your case, you have large temperature differencenMarch 9, 2021 at 12:19 pmmichutorresSubscriberOk I introduced the density as a polynomial function. For the viscosity and heat capacity I did the same but the plot was not available. nIs this a problem?nby the way, I changed to laminar and introduced the density as a function and the error of floating point exception continues appearing...nwhat can I do?nMarch 9, 2021 at 7:26 pmYasserSelimaSubscriberNot a problem. nThe floating point exception can occur because of many many reasons. Defining the density as a function of temperature or not, might not be one of these reason. It is a matter of defining the physics of the problem.nDo transient simulation and decrease the time step to a very small value and increase the number of iterations to more than 100. Run few time steps with this conditions. If you get floating point excption, you will need to refine the mesh and try againnMarch 9, 2021 at 7:36 pmmichutorresSubscriberOk thank you.ni will try the following:nnumber of time steps 20ntime step size: 0.00001nmax iterations 150ni will run this few times.nthat would be correct?.by the way, in Methods I selected Scheme=PISO, pressure= PRESTO, Momentum = Third Order Muscl and Energy =Third Order Muscl. nCould it be this the problem?nThank youMarch 9, 2021 at 7:44 pmYasserSelimaSubscriberincrease the number of iterations.nUse first order when applicable. This helps getting convergencenMarch 11, 2021 at 2:59 pmmichutorresSubscriberHi,nI changed the Method using First Orders and I set up the Run Calculation like this:nNow the Scaled Residuals looks better but everytime that it says ‘solution is converged’ I can see a peak in the plot. Is it normal? nnIf this is normal, which is my next step? You told me to use adaptive time step and let the fluent decide the optimum size. How can I do this?nmany thanksnMarch 11, 2021 at 3:45 pmRobAnsys EmployeeThat's normal, the residual will spike for each time step and then converge. As you're changing the material density where does the extra volume go in your model? nMarch 11, 2021 at 3:53 pmmichutorresSubscriberHi Rob,nI changed the Run Calculation parameters as I want to simulate 30 minutes (1800 seconds):nNumber of Time Steps: 1800000nTime Step Size (s): 0.001nMax Iterations/Time Step: 20nBut the residuals increase:nSo, I don't know which parameters should I set in order to simulate 1800 seconds.nnConcerning the material density change, I didn't think about the extra volumen that will appear. How can I consider this extra volume in Ansys Fluent?nThank younMarch 11, 2021 at 5:41 pmRobAnsys EmployeeIf you're not converging the time steps you most likely need to decrease the time step, failure to converge the step will result in the data becoming increasingly inaccurate. nRe the extra volume, you could use VOF and allow the liquid to expand into an open gas space, or for ease you can also just add a flow boundary and monitor how much mass you lose. Remember to turn on gravity! nMarch 11, 2021 at 10:22 pmmichutorresSubscriber1) As far as I know, I need to 'play' with time step size and iteration to reach convergence. With time step=0.0001s and 250 iterations, solution converges. But if I increase time step to 0.001s keeping 250 iterations, residuals become crazy. That means that if I want to decrease time step I should increase iterations? With these values the simulation will take too much time (I need to simulate 1800 seconds).n2) What do you mean with a flow boundary? Can you give me an example? And how do I know how much mass will be lost?n3) I set a heat flux in a boundary condition (wall). Should I enable the shell conductivity?nMarch 13, 2021 at 7:33 ammichutorresSubscriberHi,nHow can I add a flow boundary and monitor how much mass I lose in order to consider the extra volume?nThank younMarch 13, 2021 at 11:57 amYasserSelimaSubscriberHe meant by making the top surface outlet pressure, you can monitor the amount of mass going out.nTo use Adaptive time step, in your posted photo of the calculation tab, Do you see the word Fixed? change it to adaptivenMarch 13, 2021 at 12:03 pmmichutorresSubscriberThe amount of mass going out is something that I have to calculate and introduce in the pressure outlet boundary condition?nMarch 13, 2021 at 1:32 pmYasserSelimaSubscriberNo, you can monitor the mass flow on the boundarynMarch 13, 2021 at 3:08 pmmichutorresSubscriberWhat do you mean with monitor the mass flow?nMarch 13, 2021 at 4:15 pmYasserSelimaSubscriberreport definition - area integral - mass flux .. and select the surface .. check plotnMarch 13, 2021 at 6:32 pmmichutorresSubscribercreating the pressure outlet boundary condition and then monitoring the mass flow is mandatory? nor I can leave it as it is without considering the extra volumenMarch 13, 2021 at 6:40 pmYasserSelimaSubscriberYou can leave it. I am just explaining what was suggested by Rob.nMarch 15, 2021 at 2:59 pmRobAnsys EmployeeYou want to converge each time step in 10-15 iterations, otherwise you risk needing many more iterations to reach the end time for your calculation. There is no need to consider fluid expansion, but if the density varies with temperature the extra volume has to go somewhere. nMarch 17, 2021 at 8:26 ammichutorresSubscriberHi,nlook at my residuals. Do you think they are too high to obtain a good results?nBy the way, I ran the simulation with adaptive method and it goes really slow... In 10 hours of real life, the simulation is now at 11 seconds (it has to reach 1800 seconds). How can I improve this (make it quicker)?nnMarch 17, 2021 at 3:56 pmRobAnsys EmployeeThat residual is way too high, you're aiming for 0.001 or so. Roughly how long does it take the flow to cross one cell? nMarch 18, 2021 at 11:21 ammichutorresSubscriberHi,nI got some results on my project. Remeber that my project consists on the heating and melting of adhesive because of a heat flux inside the deposit.nnThis graph corresponds to the evolution of temperature of a point of one deposit wall and it is ok because in real life it takes 600 seconds to reach 150 ºC = 423K. At this temperature we turn off and turn on the heat flux so that it acts like a thermostate.nThe problem that I am having is that the temperature of a point in the adhesive body don't reach 423K as it is supposed. In real life, the melting of the adhesive takes less than 1800 seconds (30 minutes). What can I change in Fluent so that I get valid results for the adhesive temperature graph?nThank younMarch 18, 2021 at 2:40 pmRobAnsys EmployeeWhere is the point? Remember as the adhesive starts to melt that convection currents will start up which may increase heat transfer within the fluid zone. nMarch 18, 2021 at 2:45 pmmichutorresSubscriberThe point it is in the middle of the adhesive part.nThe adhesive melting temperature is 105?C (378K). We can see in the previous graphics that the adhesive temperature goes from 26 ?C (300K) to 67?C (340K) in 30 minutes. Something is wrong here.nViewing 36 reply threads
Ansys Innovation Space
- You must be logged in to reply to this topic.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.Trending discussions
- Suppress Fluent to open with GUI while performing in journal file
- Floating point exception in Fluent
- What are the differences between CFX and Fluent?
- Heat transfer coefficient
- Getting graph and tabular data from result in workbench mechanical
- The solver failed with a non-zero exit code of : 2
- Difference between K-epsilon and K-omega Turbulence Model
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- error in cfd post
© 2023 Copyright ANSYS, Inc. All rights reserved.Ansys does not support the usage of unauthorized Ansys software. Please visit www.ansys.com to obtain an official distribution.