Simulation Mechanical Forums (Read-Only)
Welcome to Autodesk’s Simulation Mechanical Forums. Share your knowledge, ask questions, and explore popular Simulation Mechanical topics.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Thermal analysis load parameter for a induction heater usage

3 REPLIES 3
Reply
Message 1 of 4
subbbu
698 Views, 3 Replies

Thermal analysis load parameter for a induction heater usage

Hello, 

 

I have a hollow culinder . OD 16 foot. To weld some metal on the OD, I intend to heat this shell. I plan to apply 35KW induction heatrs in the inside. Maximum available temperature = 500 F . So when the outer surface of the cylinder reached 500 F, the thermocouples automatically cut the 35KW supply off.

 

My goal is to :

 

FInd how long will it take to heat the OD if induction coils placed on the surface along the ID ? or how long will the OD take to get to 500 F

 

My approaches:

Approach # 1

In AutoDesk SImulation, I selected the inner surface of the cylinder and used the controlled temperature option and set it to 500 F. Is this method right ? In addition to this , do I have to give anything more? What is the thermal stiffness of steel ?

 

Appraoch 2 # 

I select outter face of cylinder and and subjected it to CONVECTION (free air). inner face -> same as described above. Results didnt  match prior experimental data.

 

Approach 3 #

Used the internal heat generation option. Applied 35KW across the volume that was taking the load. These results also did not match previous existing data.

 

 

 

Doubts :

 

  • Is there a way to do this ?
  • Are my approached wrong ? Am I selecting the wrong options ?
  • Should I be using any other option
3 REPLIES 3
Message 2 of 4
AstroJohnPE
in reply to: subbbu

 

Hi subbbu,

 

I do not know the physics of induction heating very well, but approach 3 sounds the best to me. You know the power input (35 KW) but nothing about the temperature that it creates on the inside or throughout the thickness. Whether you use internal heat generation or a heat flux to the surface depends on the physics.

 

Here are some things to consider.

  1. What is the thickness of the shell?
  2. What is the material of the shell?
  3. How much area is being heated?
  4. Is the heat generation uniform or a (2D?) profile? How accurately did you model this?
  5. What type of elements are you using in the model?
  6. What type of analysis are you using? (Just want to make sure 😉 Is the time step small enough to capture the dynamics?
  7. I assume that the shell begins at ambient temperature and is heated to 500 F. Over this temperature range, the convection can change drastically. You should use a temperature dependent convection coefficient and calculate what the convection value is versus temperature.
  8. Radiation can also be important at high temperature. Did you include radiation from the outside to the environment? If you are heating a small region on the inside, body-to-body radiation from one side of the shell to another side can be an important cooling effect. Did you include this?
  9. What are the experimental results?
  10. What are the calculated results?
Message 3 of 4
subbbu
in reply to: AstroJohnPE

Hello John,

 

Thanks for getting back. 
Answering your questions :

 

Temperature wise : all we know is that the system has to be maintained at 500 degree F .

 

Questions 1-2 and 4-5 : Since the model was made in Inventor, all properties were taken from there. Model is very accurate. its a 3D model and brick elements.

Questions 3 : When I did, internal heat egenration (units being Watts/m^3); I had split the solids where the heats were to be applied. When I tried the runs with HEAT SOURCE option, I had split the surfaces on which the heat was to be applied.

Question 6 : its for 400000 seconds. (yes ! 400 thousand seconds) from prior experience in the shop, we know that it takes around 2-3 days to heat it. and its TRANSIENT HEAT analysis. The software did ask us if the time is that large, we subscribed to "YES" option. The time step was set to 1

Question 7 : I quite didnt follow, John, the latter part your question. The ambient was set to SHOP TEMPERATURE : 65 degree F. So before the analysis begun, we change used the "OPTIONS" tab in "EDIT ANALYSIS PARAMETER and set to 65 degree F. the curve was set to time depenedent and at 400000 seconds, multiplier was 1.

Question 8 : I did not include radiation. I will do little digging on this. I was under the impression that radiation may not be possible. I didnt have the radiation factor too

Question 9 : experimental results : to attain 500 degree F it should take 2-3 days... around 50 hrs or so or more. 

Question 10: calculated results : attains in less than a day. (not possible)

 

I would like to indclude : I tried another approach. Using HEAT SOURCE in units Watts / m^2 . So I divided the curved surface area and gave the inputs properly. The results did kind of matched or should say is SATISFACTORY.

 

It took around 60 hours. However, I am wondering if that is the right approach.

 

Secondly,

 

  1. is there a way to limit a surface to a desire temperature ? Eg, in my case, on the internal surfaces i am applying heat source. on the external surface I am choosing convention source . But at the same time I would like to limit it to 500 degree F . Is that possible ?
  2. Also, what is the thermal stiffness of steel ? COuldnt find that on the net 

 

Message 4 of 4
AstroJohnPE
in reply to: subbbu

 

It sounds like the geometry is setup properly with the split parts and surfaces. That's good.

 

I recently performed some transient analyses in which the model was heated over 30 to 50 hours. I found that a time step of 180 seconds was good for preliminary runs and 60 seconds for a time step was good for the final runs. In my case, the model heats so slowly that a smaller time step did not increase the accuracy. You may be able to do something similar but would need to do some tests to see what time steps are acceptable. It should decrease your analysis time considerably.

 

For question 7, I agree that the ambient TEMPERATURE can remain constant at 65 F. Your load should be a convection load in which case you need to enter a convection coefficient. If the air in the shop is stationary (no fans blowing, no wind blowing through the shop), then you have a natural convection situation. The convection coefficient when the shell is at 70 F is a lot different (on the order of 0.5 W/m^2 C) than when the shell is heated to 500 F (on the order of 10 W/m^2 C). If you knew what the shell temperature would be versus time, then you could calculate the convection coefficient at different times and enter that using a load curve. If you do not know how the outside shell temperature changes with time, then you can use the option of "Temperature dependent convection coefficient" which lets you enter a table of convection coefficient versus calculated temperature.

 

My guess is that you will find that radiation is an important effect to include. It will cool the model more efficiently than the convection as the surface gets hot. And although body-to-body radiation would be more accurate on the inside surface than the "regular" surface radiation, I would try to approximate the radiation using surface radiation on the inside (and outside). If the area being heated is small -- so that the area is approximately "flat" compared to the 16 foot diameter, the surface radiation should be acceptable. If the area is large -- such as a 90 degree segment of the perimeter, then some of the hot area can "see" (radiate) to the other hot areas, so body-to-body radiation become a little more important.

 

To answer your new questions,

 

1) You cannot have the analysis stop when something reaches a target temperature. About the best you can do is monitor the results and stop it manually. If you wanted to simulate the thermostat shutting off the power, you can do a restart analysis and begin this second analysis at a chosen timestep from the first analysis.

 

2) If the "thermal stiffness" is an input for the controlled temperature, the value you are looking for is not the thermal stiffness of steel. The thermal stiffness of a controlled temperature is a measure of how effective the devide adds or removes the heat. (Technically, the thermal stiffness is equivalent to a convection coefficient times the area surrounding the node.) If my memory is correct, the documentation suggests using a thermal stiffness of 100 to 1000 times the conductivity of the material they are attached to. I suggest at least 1000 times the conductivity in your case -- just to be safe that the calculation follows the control temperature.

 

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report