Need help for Thermal stress simulation

[Anonymous]

hello, 

Can someone help me with this thermal stress simulation.

Problem : I am unable to constrain model in a way where constrains dont produce artifical stress. Where ever i put constraints i have high stress.

Can someone help me and explain me how to do this right way.

If possible can someone run simulation for me and explain to me how to setup this.

i am attaching file here and explaining scenario.

Pull force : 16.53 lb pound force

weight on the top bar : 8.81 lb pound weight

Temprature of the whole frame : 400 C

Material : Iron Cast

Scenario 1 : i want to hold this frame from one side and pull from other side with the force of 16.53 lb pound force with weight on the top on the middle bar 8.81 lb pound  with frame temprature at 400C material is Iron cast.

Scenario 2 : i want this frame to be pulled from both side with the total force of 16.53 lb pound force with weight on the on top on the middle bar 8.81 pound with frame temprature 400c material Iron Cast

Problem : where i put constriants pressure comes at 1500MPa / over 2000 MPa / over 3000 MPa and even more

i am new and learning about simulation. i have tried constriants at many different point but still didnt manage to have successful results.

Can someone please perform simulation for me and teach me how to set up this properly. how to use constriants in thermal stress study where constriant dont cause stress at any point.

[John_Holtz]

Hi @Anonymous 

We will be glad to help. Please provide the model that is setup for the simulation. (The model that you attached has no simulation setup. You have already done 98% to 100% of the work. There is no reason for someone to reproduce all of that. 🙂)

Scenario 1 and 2 are virtually the same. If you apply 16 pounds on one side, there will be a 16 pound reaction on the other side (either from the constraint or from another applied force). Since a static analysis requires a statically stable analysis, this means that scenario 1 with the constraint is the better option.

The constraints need to duplicate the reality -- at least as accurately as possible. If the constraints are accurate and the high stress occurs at only a few isolated points (often at a corner), then you just need to ignore that high value. If you are trying to model something that is true unconstrained, then you should be able to select 3 different faces (1,2,3) and apply X, Y, Z constraint to each face. See the image below. This prevents the model from moving like a rigid body but provides the least amount of restriction. (Actually, you could select 3 edges and apply similar constraints.)

X symmetry means to constrain UX, and so on.

Also, if the temperature load does not create a stress (meaning if the part is free to expand), then there is hardly any reason to apply a temperature load. The only thing the temperature load is doing is causes a small amount of displacement. If that small expansion can be ignored, then just do a static stress analysis to keep things simple.

[Anonymous]

Thanks for your time and response.

i have attached file with simulation setup please have a look.

the reason i have put two scenarios is because when holding and pulling from other side, i have huge stress at one side and little stress on other side. so i have 2nd scenario where force is applied in opposite direction in hope to achive pull effect.

Reason for appling temperature on the frame is to see what difference it make on the frame in  terms of strength, as i have tested this frame in static stress simulation.

I will really appreciate if you explain constraints on the frame which i have attached with reference number on the frame please have a look at attached file. i Want to make a request if possible for you please can you try this simulation and show me how to do it, because i am failing to perform or understand this simulation.

I am really strugling to understand how to perform this thermal stress simulation.

i want to know how to constrain this frame that causes no artifical stress.

Material of Frame is Iron Cast.

please see attached files 

[John_Holtz]

Hi,

Here are a couple of thoughts before I forget.

1. There is an option under "Manage > Settings > General > Remove rigid body modes" which is useful for situations where the model is under constrained. It might be useful in your situation, but it has some tight requirements in order for it to be used properly. (See this page for more information: http://help.autodesk.com/view/fusion360/ENU/?guid=SIM-RIGID-BODY-MODE-GUIDE-CONCEPT). I find it just as easy to apply constraints, and that gives me a feeling that I know what the analysis is doing.
2. You mentioned the temperature reducing the strength. None of that is part of the analysis. The material properties are what you enter (which must be based on the anticipated temperature of the material). You can apply a temperature of a million degrees, and the strength is what you entered. (Actually, a linear static stress analysis does not care about the allowable limits, other than reporting the factor of safety, so the results can go up to a million psi.)

I am still not clear what the real constraints are, if any. Since you mentioned applying equal and opposite loads, I will assume that there are no constraints in real life (other than someone or something holding the frame and pulling on it). The following constraints are inspired by the fact that the model, loads, and results are symmetric. If you would slice your model in the YZ plane through the middle, you could actually analyze half of the model and get the same results.

See the attached image to better understand the description of my constraints. Also keep in mind that constraints are to prevent the model from translating in X, Y, Z (UX, UY, UZ) and rotating about X, Y, Z (RX, RY, RZ).

1. If the model were sliced, you would apply a symmetry constraint to the cut face. That is, UX is fixed. Although your model is not sliced, selecting the edge A-C and applying a UX constraint makes it behave similarly. This limits the model in UX and RY motions, but the other 4 motions would still be free. (Restricted motion in UX should be obvious. If you think about trying to rotate the model about any Y axis, that is also restricted because the nodes on edge A-C would need to translate in the X direction in order to rotate the frame about the Y axis, and the UX constraint prevents that.)
2. The vertical (Y direction) and front-to-back motion (Z direction) can be measured from any point in real life. If edge A-B were fixed in UY and UZ, that provide that "measurement point" and would prevent motion of the model in 5 directions. The model would only be free to rotate about RX. (Specifically, it can rotate about an X axis that passes through the edge A-B because no other constraint yet prevents that rotation.) Note that applying UY to this edge implies that the bar is not going to bend across the 3 mm width. In other words, line A-B does not bend. This is not true in reality but probably very close to reality given the small size. (If the calculated stress is high, you will know this constraint is wrong.)
3. To prevent the model from rotating about the X axis passing though edge A-B, constrain any other point in the model in Y translation. Point C is a good choice for the UY constraint.

I just realized that I made a mistake with the UY constraint, but I am too far into it to change now. 🙄 In my setup, the X reaction forces will be close to 0 because the applied forces are equal and opposite. The Z reaction forces will be close to 0 because there is no load in the Z direction and no twisting that would cause a reactionary moment. The vertical reaction force would appear at the constraints in step 2, and that is a problem. (And this is why you check all of the results: displacement, stress, reactions, etc. Just because 2 of them look reasonable doesn't mean that all of them are reasonable!)

Depending on how the 8 lb vertical load is resisted, it may be better to apply half of the load to each "arm" of the frame (the same location where the 16 lb loads are applied). Then if the Y reaction force due to the constraints applied in step 2 will be close to 0, and the result will be successful. As it is with the above constraints, the 8 lb vertical load is resisted at the front and back of the top bar which is not realistic.

If this frame is resting on a table, some of the nodes on the bottom of the frame will contact the table, and the displacement will cause other nodes to lift off of the surface. In this case, you would model the table and use separation contact. (Frictionless or UY constraint on the bottom surface would imply that the frame cannot lift off of the table, and that would not be realistic.)

Sorry to be long winded, but I hope it helps.

[Anonymous]

hello john, i really really appreciate to the length you go and make effort to explain and solve problems. i have seen your replys on the fourms before as well.  I want to thankyou for your time and effort. Sorry for late reply because i was testing frame with your guide. wanted to test and ask you any question i have after that.

Following your guide now frame displaces the sameway i wanted. Stress for the very first time came down from less than 400MPa. this is great however i still have questions i want to ask.

I want to explain scenario to make sense of what i am trying to learn and achive.

Frame is made of Iron Cast Metal. Let suppose at room temprature it will take 10 kg force to bend this frame. Now if metal temprature increased it should take less force to bend frame. If iron cast melt around 1204C, then reaching teamprature around 800C or near melting point it should take less force to bend this frame. I hope you get idea from this what i am trying to see in simulation.

I have tried higher temprature but result is same with 400C and 800C. is this the right simulation to achive this?

is somthing wrong i am doing in this simulation? How to see deformation effect on the metal when temprature is applied?

Please Have a look at attached images. i have seen the frame streching (or free to move) in the Z direction, is it normal in Thermal Stress simulation? does it effects results? When i check DOF it says potentially fixed, is it ok this way, does it effect results?

I have attached result image with 800C applied which have same results as 400C.

[John_Holtz]

Hi @Anonymous 

You need to enter the material properties that are appropriate for the temperature. The modulus of elasticity (Young's modulus) is lower at higher temperature. 

[Anonymous]

it means temperature in the simulation enviorment will not weak metal but will only show stresses caused by temperature.

in a way if i change material properties in static stress test(strength of the material according to temperature change) it will have same result? as if i wanted to know what will be the strength of the material at 800C? if applied force of 10 kg.

If material yeild strength is changed in the properties. will it have same effect of metal getting weak in terms of bending. can i simulate this way?

[John_Holtz]

The temperature does not change the material properties in the simulation. To get accurate results when the model is at an elevated temperature, you need to enter the material properties that correspond to the elevated temperature. (Of course, the same is true when the temperature is much lower than room temperature.) In other words, the materials properties that are used in the analysis must match the material properties that occur in real life. Using material properties from room temperature in an analysis will not match a real life situation at 800 C.

The displacement is 99% based on the material property of Young's modulus (also known as modulus of elasticity). Changing the other material properties will not change the amount of bending. You can demonstrate this by .... changing the material properties and seeing what happens. (The Poisson's ratio has a smaller effect on the displacement.) If sounds like your design is limited by the displacement. In this case, change the Young's modulus.

The yield strength is only used to calculate the factor of safety. The other results (stress, displacement, reaction force) are not changed by the yield strength. The same is true for the ultimate strength.

[Anonymous]

Thankyou soo much john, you have cleared alot of questions in my mind and you have been really helpfull through discussion. One thing i understand now is that i dont know alot of stuff about simulation that i have to learn. I am new to simulation and interested in learning about simulation. I was unable to figure out few thing after watching videos and reading online, but your explanation cleared alot of questions.

Once again Thankyou for your help.