stages of loadings on fusion

[andres_urrutia]

hi everybody.
 
is there any way to add loading stages on Fusion360?
I'm modeling an horizontal vessel which is submited to a temperature that tend to enlarge the equipment. there are frictional saddles but I need to solve first the vertical loads to actívate the fricctional resistance, then i might run the termal effect because i need make interact expansive termal loads with friccional resistance of every saddle.
may I have explained well? is difficult to me to express this idea on english.

best regards and happy new year

[James.Youmatz]

Hi @andres_urrutia ,

Thanks for posting. I think I understand - but want to clarify a few points.  Is the vessel in contact with the saddles before it expands? 

Is it possible to share the model with me so I can see first hand how you are loading this vessel?

Thanks,

[andres_urrutia]

sure.

I've attached the model in the link below

https://a360.co/2LFykzl

[James.Youmatz]

Hi @andres_urrutia ,

The link does not have the download option available. Can you toggle this to on? 

Based on what I can see in the viewer though, it looks as if the saddles are touching the vessel. In this case, what I would do is run a thermal stress analysis - with the contact faces of the saddle and the vessel set to separation or sliding contact, with the friction defined. 

[andres_urrutia]

thank you. I have modified

https://a360.co/2LFykzl

[James.Youmatz]

Hi @andres_urrutia ,

Looking at the file now. It looks like you have modified the set up to include the separation contact between the vessel and the supports. I also see the friction values. 

I just hit solve, but it will take some time. Are you not seeing the correct/intended results? I'm not sure what the issue is here just yet.

[andres_urrutia]

thank you James.

the problem is the following:

I understand that the friction contact might work when the normal load (gravitational load in this case) are present in the contact.

when the análisis is being performed, if the analysis is being done under one stage, the forces and temperatura vector Will by applied at the same time so the proportion of forces present to actívate the friction resistance of the saddle Support Will be not enoug to add some restriction to the problem.

the result of this simulation looks like that the saddle supports are just sliding supports… and why? because the temperatura is acting at the same time with the gravitational loads (which are responsable to generate the normal load neccesary to actívate the friccional restriction). 

[John_Holtz]

Hi @andres_urrutia 

I am helping James with your questions. But first, I have some questions about your model about how things are connected together. For example,

1. You have a tank sitting on many saddles. Is the tank welded to the saddles, or is the tank sliding in the saddles?
2. The many saddles are sitting on pedestals. Do the saddles slide on the pedestal, or are the saddles connected (by weld or bolts) to the pedestals?

To answer some of your questions,

1. The calculation is based on all of the loads applied. There is no option to apply one load first, then another load, then another load. Mathematically, the result is the same. The normal force where the parts are sliding is the same with all loads applied simultaneously compared to if you could apply the gravity first.
2. If the friction is not enough to prevent sliding, then the parts will slide. The solution to a sliding problem is a dynamic analysis: the distance that something slides before stopping requires time and inertia. So a static analysis will not include friction when the parts slide.
3. A thermal stress analysis runs a steady state heat transfer analysis followed by a stress analysis (that includes the temperature results). The heat transfer analysis requires a source of heat  and the removal of the heat. You only have a constant temperature applied. I am not sure if the heat transfer analysis will solve that properly. (I will do a test.)

An alternative solution to the friction problem would be as follows. (My description is assuming that the tank is welded to the saddles, and the saddles slide on the pedestals.)

• Suppress the pedestals.
• Apply constraints to the bottom of the saddles that prevents them from moving vertically.
• Run the analysis.
• Get the reaction force at each saddle.
• Add a "friction" force to the bottom of each saddle equal to the reaction force times the coefficient of friction.
• Run the analysis.
• If the saddles still "slide" in the expansion direction, you know the friction is not enough to prevent the thermal expansion. If the saddles "slide" in the reverse direction, you know the friction force is larger than reality.

Let me do some more work on these ideas.

[John_Holtz]

Hi again @andres_urrutia 

I did a test model for the thermal stress. The analysis will run with just a temperature load applied.

HOWEVER, you only have temperature applied to SOME of the parts. There is a good chance that the parts without an assigned temperature are at 0 C. With a stress-free temperature of 20 C, this would cause all of those parts to contract. That is probably not what you want.

[andres_urrutia]

right, the saddles are welded, that is why I have defined a bonded contact.

the pedestals are set to get a surface to apply a "frictional contact".

according to my knowledge about iterations problems is the following:

I understant that the software, in oder to ensure the convergence, wil divide the load vector in "steps" so at the first step the model Will solve the problem with part of the total effect of temperature and part of the total weight… then the friccional contact Will check if the product of the reaction and the coefficient (0,3) is less tan the force due to the termal expansión. the most probable situation is that the product Will be less tan the expansión force and finally the stifness matrix Will asume zero stifness and the saddle wil move. then during the second step, the analysis Will be get the same situation and this Will be the same situation during all the steps up to the end of the analysis. 

for the other side, if we perform first the gravitational analysis, the matrix stiffness Will consider the sddles as a restrained elements because the product between the reaction and the coefficient Will be high, then as a second stage we start loading the termal effect, during the first steps is probable that the equivalent force of the expansión due to termal effect Will be not enoug to reléase the saddle and maybe during the last steps the situation can change and the saddles begins to move. clearly the result must be different, but I think that the second case is more realistic.

[John_Holtz]

Hi @andres_urrutia 

You description is correct for a nonlinear analysis but wrong for a linear analysis. The thermal stress analysis is a linear analysis. 

• In a nonlinear analysis, the loads are applied in steps from 0% to 100%, and the results are calculated at each step.
• In a linear analysis, the loads are applied in one step (100%).
• However, if the system is really linear  and static -- meaning small displacement and the stiffness does not change and there is no acceleration of the model -- then there is no difference between applying the loads all at one time (100%), or applying gravity first and then applying the other loads. At 100% load, the friction force = gravity*mass*coefficient of friction, and that load is added to the thermal load. If you could apply gravity first and then the thermal, the last step would be = gravity*mass*coefficient of friction + thermal load. They are the same.

What you may be thinking is that an analysis with separation contact is an iterative solution, so there are "steps" involved in the analysis. But the "steps" are to determine which nodes are in contact and which nodes have separated due to all of the loads. The solver cannot know which nodes have separated until it calculates the displacements, and it cannot calculate the displacements without knowing which nodes have separated. It requires an iterative solution to find the displacements and which nodes have separated.

[John_Holtz]

Hi @andres_urrutia 

I wanted to follow up with you to see if you had any remaining concerns or questions regarding your ongoing case.

[andres_urrutia]

thank you John.

so, there is no solution for this problem?

thank you anyway. your answers are very clear.

[John_Holtz]

Hello,

I want to make sure that I have not missed something in our conversation, so let me summarize my understanding.

1. The original question was whether Fusion could perform the analysis in stages: stage 1 includes the gravity load, stage 2 includes the thermal loads, and so on. The answer to that question is no.
2. The reason for your original question is because you felt that the friction forces had not developed, and therefore the thermal loads caused the vessel to slide. The answer to that question is the following: that is incorrect assumption and is not necessary in a linear analysis. You can think of a linear analysis as using the method of superposition. It does not matter which loads are "applied" first and which come second. Only the end solution with all loads is calculated. So the result with having the friction forces first and the temperature load second are identical to having the temperature load first and the friction force second.
3. Then why does the vessel slide? My guess is that the friction is too small to resist the thermal load. When that occurs, the analysis lets the model slide "freely". The way to verify this is to apply a constraint that prevents sliding motion, and then check the horizontal force against the friction force.

Have I missed something?

(Regarding item 3. In my opinion, setting the friction to 0 when the part slides is the wrong method. This is the method used in the two solvers that I am familiar with: Nastran and Simulation Mechanical. If the friction is too small, the solution should be the maximum friction force applied at the position that the static model stops, instead of using a friction force of "0". I do agree that if it slides, the dynamic friction becomes important instead of the static friction, but that is not what most users are trying to analyze. I wrote "freely" and "0" with quotes " " because what Nastran does is more complex than using a friction of 0. In case you did not know this, the solvers used in a Fusion simulation are the Autodesk Nastran solvers.)

[andres_urrutia]

thank you John for your explanation.

the problem that we want to solve is to determine if the movements of the saddles Will occur.

i really don't understand well how can we solve a linear problem (thermal) with non linear contacts like frictional ones.

I'm asking that because in other non linear softwares you can set the time of every load and the convergence of the problem is better compared to the analysis if you don't do it.

in this case I'm convinced that the problem Will be different if we start the gravitational loads and with this, the normal load and as a consequence the frictional resistance of every saddle, then  we apply a termal load (as a second stage).

[John_Holtz]

Hi @andres_urrutia 

In theory, a linear stress analysis can handle contact with friction just as easily as it can handle contact without friction. Both require an iterative solution.

The question is whether Nastran supports friction in a linear analysis. The Fusion interface implies that it should. I am trying to confirm if it really supports friction or not.

If I were you, I would use the suggestions that I provided previously (using a constraint or force) to simulate the friction so that you can complete your analysis.