Type of contacts in static structural

  • 82 Views
  • Last Post 3 days ago
Francisco Guerra posted this 2 weeks ago

Hello to everyone, I'm using workbench 18.2, static structural, to obtain the v-m stresses and the total deformation of an index finger that belong to a hand orthosis model. 

As boundary conditions, there is gravity, a force (22N) that represent the flexor tendon (nylon line) and a fixed support located in the pin that joins the finger with the rest of the hand orthosis.

My model have 3 phalanges that are joined together across 3 pins (these phalanges should rotate when a nylon line pulls from the finger tip alog the finger). I don't know if default ANSYS bonded contact is the right setting for the analysis or maybe another one like frictionless (between phalanges and pins), frictional, etc.?. Maybe I have to add some joints into model?

 

 

Thank you for your help and support.

Order By: Standard | Newest | Votes
peteroznewman posted this 2 weeks ago

Hello Francisco,

Thanks for writing a fairly detailed question!

Bonded contact is not useful when you have large relative motion between two solid bodies. It's for when you want to "glue" two bodies together. One way you would use Bonded contact is to glue a pin to one part, while the adjacent part that has a hole that the pin also goes through has frictional contact.

Frictional contact is useful when you want large relative motion between two solid bodies. However, frictional contact requires very careful use to get a solution.

For a pin connecting two parts to make a hinge, there is another way to connect the two parts that does not use contact. It is called a Joint and models that use joints instead of frictional contact are much easier to solve.  The type of joint that makes a hinge is called a Revolute joint. To use it, you don't actually need the pin. You use the cylindrical faces of the holes on one part and call that the Mobile side of the joint then use the cylindrical faces of the holes on the other part that the pin went through and call that the Reference side of the joint. I recommend you build your first model with joints.

The nylon cord has tension, but what in the model is the tension pulling against?  There has to be some spring or some part that gets compressed and provides a resistance to the tension in the cord, and that compressive force would straighten the finder when the tension in the cord is relaxed. What is providing the restoring force?

Here is a video tutorial on Joints.

 

Francisco Guerra posted this 2 weeks ago

Hello Peter,

First of all, thank you for your time to gave me an answer and also I'm sorry for mi late reply but I was reading a lot about configurations and expend a lot of time doing simulations today. I read everything you said and also made some modifications to my analysis but still continue giving me some problems. I've tryed your recommendation in the following order:

1. I changed some bonded contacts to frictional (0,2,augmented lagrange and adjust to touch) and I leave only 2 of them as bonded (the middle and right phalanges with their respective pins)... after 4 attemps of 1h every simulation, doesn't work.

2. I deleted all bonded contacts with the exception of 2 of them (lateral contacts between left and middle phalanges and lateral contacts for the middle and right phalanges). Then I created revolute joins body to body (between phalanges and the pins)... after many attemps moving configurations with a total of 3h, doesn't work.

3. All contacts deleted, I worked only with revolute joins without the pins using the cylindrical faces as you said... after many attemps with a total of 3 hh, doesn't work.

I don't know if maybe the problem is due to the force of 22N that represent the flexor tendon, maybe is not properly restricted or bounded. You asked me about the tension pulling against the nylon cord, to anwer that, let me tell you that the project involve the use of mini servomotors, so when the servo pulley rotate counterwise he is pulling from the tip finger from the down side, producing the flexion effect, at the opposite side, when the servo pulley rotate clockwise he is pulling the tip finger from the up side, producing the extension effect. Below you will find some images that I prepared to show you, for better understanding of the situation.

 

Finally, some of the errors that many simulations gave me was: 1. an internal solution magnitude was exceed 2. one or more MPC contact regions or remote boundary conditions may have conflicts 3. The unconverged solution is output for analysis debug purpose 4. The solver engine was unable to converge, etc.

I know the v-m stresses and the total deformation of the pins and phalanges are wrong using all bonded contacts, but this situation was the only one in which there was convergence.

Maybe I have to include both nylon lines from the finger tip across the entire finger? Will be possible for you to check my analysis? Attached you will find all the project. I uploaded to wetransfer: https://we.tl/t-qfWi7L3KIw 

Please I kindly request your support again.

Thank you Peter.

 

  • Liked by
  • peteroznewman
jj77 posted this 1 weeks ago

Without looking in to much detail (do not have the time currently), this is a linked mechanism that is unstable, basically as a triple pendulum, if you add gravity to it. As you suggest you would definitely need to add some form of stabilisation mechanism, perhaps as you suggest by adding these tendons/cables. Thus when the metal parts are being pushed down they (cables) will take/resist some of that through tension.

Francisco Guerra posted this 6 days ago

Hello friends, thank you for all your commentaries and recommendations.

The problem after all was the material: ABS . I used the same ABS data from ANSYS 19.1 (Engineering Data), that were posted by peteroznewman in other topic here in the forum, but in ANSYS 18.2 (Workbench, Static Structural) the program can't converge with the conditions and boundaries that I posted previously.

I changed completely the material to Structural Steel and also to SS304 (this material was added directly to the Engineering Data) and in both situations the program converged and presented the deformations and stress results without problems.

Now the big question is: Somebody know or have an idea why this is happening with ABS? Any suggestions?

Thank you,

Regards.

 

peteroznewman posted this 5 days ago

 Hello Francisco,

One reason that it might run with one material and not the other is SS304 is a lot heavier than ABS, so gravity exerts a much larger force on each body, while you have a constant 22 N horizontal load. So perhaps there is a Static Equilibrium with the SS304 while there is no Static Equilibrium with the ABS.

In any case, you don't want a manipulator that only works with gravity working in one direction. That is why you want two cables under tension. They provide the stabilization against which gravity can pull the links slightly around depending on what direction gravity is pointed.

Regards,
Peter

Francisco Guerra posted this 4 days ago

Hello Peter;

I hope everything is fine with you, because when is related to my person, well I feel a bit frustrated with this project. I know that I don't have the neccesary expertise and that's why I've been studying many papers, books and videos these days, I've tryed all your recommendations, but anyway the static structural simulations still are giving me errors, even in the last model with the two cables (flexor and extensor cables).

I know something must be wrong in the geometry, connections, forces or other, but can't find why or what... Willl be possible for you to check my simulation to see why is not working??

Thank you, kindly regards.

Attached Files

peteroznewman posted this 4 days ago

Hello Franscisco,

It's late now, but I have a copy of your file and I will take a look at it tomorrow.

Regards,
Peter

  • Liked by
  • Francisco Guerra
Francisco Guerra posted this 3 days ago

Thank you Peter for your help¡¡

Regards,

Francisco

Attached Files

peteroznewman posted this 3 days ago

Hello Francisco,

I am working on your project, but I am trying to do it on the Student license, which has node limits that your model exceeds. I was going to simplify the geometry by removing the blends, but I don't have access to the SW files.

Please create a zip archive of the SW files and attach it to your post above.

Regards,
Peter

  • Liked by
  • Francisco Guerra
Francisco Guerra posted this 3 days ago

Done Peter. Inside the zip you will find an assembly and the individuals parts, if you need something else, please let me know.

Thank you.

 

peteroznewman posted this 3 days ago

Francisco,

You don't want a solid body filled with solid elements to represent the cables. That is computationally too expensive. I am going to replace the cable solid body with a line body meshed with beam elements. These are computationally very efficient. The cables have to slide on the conical face of the hole. I am going to replace the conical holes with a blend radius. I'm going to put a force on one cable and a displacement on the other cable to cause the finger to curl a little.

What results do you want from this model, just stress in the parts?  What about how that stress changes as the finger curls up.

Regards,
Peter

Francisco Guerra posted this 3 days ago

Peter,

I'm agree with your modification for the cables if is more efficient is better. The cables (nylon) have a 1mm diameter and the holes for the wires through the finger have 1.2mm diameter, this way the cables can move inside the holes when the somebody are doing flexion or extension of the finger through the movement of the servo pulley. The holes are cylindrical with a fillet of radius 0.5mm, there is no problem with changes.

The purpose of the simulation is to know the stresses in the three phalanges of the finger made of ABS and in the pins made from SS304 (I started with SS304, probably I will change this pins also the ABS but depend if all the material or geometry of the finger can resist the forces). Deformations due to that 22N force finger flexion (or extension) also are of interest.

The stress changes in the finger due to finger curls down (or up) are also important to know, but I thought that this type of calculation was part of a dynamic analysis or not? I'm sorry if I'm wrong about this thought, any comments and information for my knowledge is well received

Thank you, Regards,

Francisco

peteroznewman posted this 3 days ago

Francisco,

This is a very challenging problem to get ANSYS to converge on the solution. The approach to very challenging problems is to simplify them as much as possible until you get a model to converge, then you can add more detail later. This is what I did to your model.

  • Made the cables beam elements
  • Replaced all the pins with revolute joints
  • Simplified the geometry (removed small blends) to reduce the node count for speed and to fit in the Student license
  • Made the first link rigid to reduce node count and fixed it to reduce the degrees of freedom in the mechanism
  • Made all the material structural steel
  • Changed the contact to have lower Normal Stiffness
  • Started with 400 substeps.
  • Added translational joints between the cable and the first link to apply the 22 N Force and a Displacement of zero in step 1, and a 1 mm displacement in step 2 to curl the finger.
  • In Solution Controls, turned on Stabilization. You can try to run it without, maybe it was not needed.

Regards,
Peter

Francisco Guerra posted this 3 days ago

Hello Peter,

Yes, I know is a very challenging problem, that's why I told you that I felt a bit frustrated with it. Thank you for all the time dedicated to teach me and for the time you spent making the problem work. I will try to get ANSYS 19 asap the check the file you attached, then I will review all your commentaries directly in the problem file and I will begin to make some changes.

Probably I will have some questions, but not before some days to understand better the resolution of the problem. 

Thank you again¡¡ Regards, 

Francisco

peteroznewman posted this 3 days ago

Hello Francisco,

I found a mistake in the model attached above, so I deleted that and attach Rev1 to this note.

I forgot to check the direction of the Translational joints and they were pointed in Z instead of X. That is fixed below.

Regards,
Peter

  • Liked by
  • Francisco Guerra
Francisco Guerra posted this 3 days ago

Peter, it seems there is no file attached.

Regards,

Francisco

peteroznewman posted this 3 days ago

Francisco,

As is often the case in nonlinear models, they are a lot more stable converging under displacement BCs than force BCs.

I changed from applying 22 N to applying a displacement that results in a 22 N reaction force. Now it is being attached.

Since the nylon is only 1 mm thick, it must be stretched 7 mm to get to 21.6 N of tension.  You can stretch it a bit more to get to 22 N.

Regards,
Peter

Attached Files

Francisco Guerra posted this 3 days ago

Thank you Peter, it´s amazing all the knowledge you have, I see why you are always helping everyone here in the forum. I will be attentive to download the file as soon as it is available.

Regards,

Francisco

Close