simulation

[Ait-Tek]

I am looking to design a Davit arm with long reach for offshore wind farm. with a few more changes I can get greater than a safety factor of 3 so no problems there. My question is how to determine the pressure on the bearings shown in red (simplified). I do have other iterations of the arm but still need to find out how to get the value for the bearing/bush. Any help would be really appreciated. I have 57 to make so need to get it right lol

[Marcin_Kosciolek]

Hi @Ait-Tek 

I understand you want to extract pressure on the faces of bearings. You can use contact pressure values from the output results. This tells us how contacting faces are "pressing" each other. To be accurate, we should also define separation contact instead of bonded, because we predict there can be some gaps if a load starts to act.

Below I attach a sample model:

https://a360.co/3BJjK1f

[Ait-Tek]

Hi Marcin,

really appreciate your assistance. I think I understood what you said and found the Offset Bonding contact. but I don't get the result I was expecting. Before I added the bearing and shaft, I ran the simulation and had a safety factor of 3.8. then I added the shaft and bearing with the off set contacts and I get a safety factor of 15 and only 0.5MPa where as your value looks more realistic. would you mind having another look at my simulation to see where I have gone wrong

Regards

Andy

[Marcin_Kosciolek]

Hi @Ait-Tek 

I noticed a strange behavior in your model. The reaction forces are not equal to the applied load. Of course, they should be in the balance. Messages from the solver suggest, that it can be also connected with curved geometry. I calculated this model in Autodesk Nastran, and there I get results, what I expect (reaction forces are also balanced).

 

I need to investigate your case more thoroughly. A nonlinear study could be a solution for that issue. I will check it out, and let you know.

Below, I attach the model from Fusion, which I adjusted, so you can see what boundary conditions and contacts I used (but as I mentioned, something is wrong with the results, and it needs to be investigated).

https://a360.co/3kX6b7m

[Marcin_Kosciolek]

Hello @Ait-Tek 

The good news, I managed to perform the simulation correctly. The troubles were generated by enabling the "Remove Rigid body modes" option. In your case, we don't need to use it, because the model is correctly supported, and we don't expect that some components can "fly away". When I deselect this option, I get much better results, and after checking reaction forces, they are balanced related to the applied load.

Here is a model with incorrect and correct results (the differences are noticeable):

https://a360.co/3kX6b7m

[Ait-Tek]

Thanks for getting back to me. Look forward to the solution

[Ait-Tek]

Thanks Mate,

had to be something silly. re-ran the simulation with a slightly increased load and got results I was expecting.

One other question. I want to apply a wind load to the side of the arm, would you simply apply a horizontal force against one face and add a UDL of 500N (seems to be a standard value for a 60MPH wind force). Thats what I have done and get a reaction from it, but just thought I would clarify.

Again, thanks for your assistance, much appreciated.

Andy

[Marcin_Kosciolek]

Hello @Ait-Tek 

I am happy that the issue is solved! Regarding the second question. The best way would be to create CFD study and obtain pressure on the faces of a model, which we can export to structural simulation. If we are not able to do this, we can simplify it, as you described, but remember it will produce less accurate results. 

[Ait-Tek]

Hi

I don't have the software for a CFD Study. I think applying a UDL on the side face should be worst case.

thanks again

PS

are there any tutorials that go through all of the functions of the software and applications similar to mine. all I find is fairly basic tutorials

[Marcin_Kosciolek]

Hi @Ait-Tek 

Your approach is right, finding the worst-case scenario and calculating that will get us on the "safe" side.

Regarding the second question. Did you check our channel on YouTube? You will find there some webinars, information about individual features, tutorials, and quick tips.

Here is a link:

https://www.youtube.com/playlist?list=PLmA_xUT-8UlJKQ4ANVugnQZEqTxD5_s2Z

Other resources of knowledge:

https://help.autodesk.com/view/fusion360/ENU/courses/AP-SETTING-UP-LINEAR-STATIC-SIMULATION

https://help.autodesk.com/view/fusion360/ENU/?guid=GUID-58159399-B08F-43BF-89E3-57AD489FF29C

I hope it will be helpful for you.

[Ait-Tek]

Thanks for the  links Ill go through those.

Another question: Manual Contacts

back to my bearings again, when in the general options selections is my "primary body" the shaft or the bearing like wise is the "secondary body" . I have been choosing the shaft as the Primary and bearing as secondary.

then I get to pick selection set 1 and 2, it only lets me select the shaft for selection set 1

and the bearing for selection set 2 

I chooses separation  and check the auto activation distance

is that the correct workflow?

then I have to apply a constrain which I use the fixed on to both bearing rings see below. again is that correct.

thanks in advance

[Marcin_Kosciolek]

Hi @Ait-Tek 

Regarding the contacts, in your case, you should already have automatic contacts between shaft and bearing. Just change the type from bonded to separation (software creates bonded contacts in locations, where various bodies are touching each other). 

I see you try to create manual contact between the shaft and the outer face of the bearing. Since we want to simulate real interactions, we should choose the inner face of the bearings, because there we will observe the interaction.

Regarding the constraints, since we have separation contact (the movement between faces is allowable), we need to be sure the model is stable. Notice please, the shaft can move along its own axis. We need to add an extra constraint, it can be an edge which I marked as red in the screen below.

[Ait-Tek]

Hi Marcin

I hope you dont mind all the questions, I do appreciate your assistance.

I think I have applied everything correct. the DFM shows the bearings are free, but I dont seem to get the the contact pressure I had before. would you mind casting your eye over my simulation attached. I am also using remote force as the load would be suspended from the arm on chain blocks.

I am showing a hollow section arm now but thing about it the material through the bending process will stretch/compress so I would know how that would be simulated so I may go back to my previous design of two side plates. but I can change that later once I know how to apply the loads and constraints accurately. 

thanks in advance

[Marcin_Kosciolek]

Hi @Ait-Tek 

As I can see, you have only one fixed support on the bottom face of the shaft. In this case, you will not get a reaction on the bearings, because they will behave like the shaft (if separation contact is defined, the bearings will slide over the shaft). You need to add additional constraints.

You can share the model, so I will check it.

[Ait-Tek]

Hi Marcin,

hope your well

Thanks for the feedback.

I have attached my model. one thing I cant seem to do is when you do "auto contact" then edit the bearings to separation I cant see how to pick the inside face of the bearing as you mentioned. but I can do it when you do the connection manually.

I have ticked the gravity box but doesn't seem to  have much affect. 

finally when the davit arm is installed, it would be lifted and dropped in to the bearing. How can I find the center of gravity to mount a lifting eye for the crane to lift that will keep the shaft vertical

Regards

Andy

[Marcin_Kosciolek]

Hi @Ait-Tek 

I am fine, thank you! Regarding the contacts, could you attach the model one more time? Cause I don't see a link to the model. 

Gravity in your case will have rather a small impact because the final load is quite high.

To find the center of gravity, you can use the tool in the design workspace called "Center of Mass" under Inspect icon.