Type of contacts in static structural

  • 888 Views
  • Last Post 04 March 2019
Francisco Guerra posted this 06 December 2018

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 06 December 2018

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 07 December 2018

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 07 December 2018

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 09 December 2018

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 10 December 2018

 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 11 December 2018

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 11 December 2018

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 11 December 2018

Thank you Peter for your help¡¡

Regards,

Francisco

Attached Files

peteroznewman posted this 11 December 2018

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 11 December 2018

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 11 December 2018

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 11 December 2018

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 12 December 2018

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 12 December 2018

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 12 December 2018

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 12 December 2018

Peter, it seems there is no file attached.

Regards,

Francisco

peteroznewman posted this 12 December 2018

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 12 December 2018

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

Francisco Guerra posted this 28 February 2019

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

Hello again Peter, I'm really really sorry for my late reply, but unfortunately I was with important health complications in the last time and recently started to work again in this project. I have some questions that I hope you can help me to solve, well I'm trying to do the same as you but I'm having troubles into represent the cables as beam element, this has to be done in space claim or design modeler?. The 2 question is what I have to do to made the first link rigid and add that inertial reference system you have in your file. The 3 question is how do you calculated that Nylon must be stretched 7 mm to get to 21.6 N of tension?. 

Please I kindly request your help and support.

I'll be waiting your commentaries, thank you.

Regards,

Francisco

peteroznewman posted this 28 February 2019

Franciso,

Sorry for your health issues.

3. If you know Young's modulus E, the cross sectional area A and the length L, you can calculate the beam axial stiffness k = AE/L  and then use x = k/F to calculate the stretch.

1. Yes you have to make beam elements in SpaceClaim or DesignModeler (where they are called Line Bodies).  Which one are you using?

2. To make a body rigid, in Mechanical, under Geometry, click on the body and in the Details window, you can change Behavior from Flexible to Rigid.

Regards, Peter

Francisco Guerra posted this 01 March 2019

Hello Peter, thank you for your concern, really appreciate it¡

Finally I did the transformation from the cables to beam elements using the extract button (prepare menu) in spaceclaim. I was able to replicate in my own file yours steps from file rev1 and got the same result, even I did the calculation using the force (22N) instead the 7mm displacement.

Now I'm trying to have the deformation in the fixed phalanx, so I changed this part from rigid to flexible and then I activated the third pin and change it from flexible to rigid to be used in the body to ground joint (in reemplacement of the phalanx), but I don't know why the stress changed from the 1 and 2 phalanges to the inner perforation for top and bottom cable in the 3 phalanx. Supossedly the stress should be remain in the phalanges included the third one.

Can you help me with this problem? I made other changes, but the results still is the same. Attached you will find the file in rev2 to see if you can see what is wrong please.

I'll be waiting your commentaries, thank you Peter.

Regards,

Francisco

Attached Files

peteroznewman posted this 02 March 2019

Franciso,

This joint has the coordinate system a long way away from the faces that create the revolute.
That is a mistake. Delete the joint and recreate it.

Francisco Guerra posted this 02 March 2019

Hi Peter, well I did everything in a new file and it worked perfectly (file A), but I have a technical question: why the traslational joint for top and bottom cable have as reference just one blend and as mobile a vertex? because I've tryed in another simulation to change the vertex by edge (all the cable) and the simulation doesn't work. In a 2 simulation I've changed the blend by all blends and areas around the cable and the simulation worked in deformation but the stress is almost zero (file B).

So why the simulation works perfectly with the cable vertex and one blend for top and bottom cable and with other changes doesn't work or doesn't show what it should be? maybe is because the vertex is already a representation off all the cable and changing this to edge it's like telling to the program that the entire cable must move through that only blend. Also why the vertex have to translate only trough one blend? because this area is the representation of all the area around the cable?

Thank you Peter,

Regards,

Francisco

 

peteroznewman posted this 02 March 2019

Hi Francisco,

You have a revolute joint defined...

but then you have Bonded Contact defined...

making the revolute joint redundant.  Carefully check all your contacts to see if they are appropriate.

There is a pernicious setting that automatically creates contacts each time you attach geometry. I prefer to turn off that feature.

Regards, Peter

Francisco Guerra posted this 02 March 2019

Peter,

I turned off the auto detect contact, because as you said this contacts were created automatically, but after delete them, there was no change in simulation, the results still are the same. Can you check just file B please.

Thank you, Regards,

Francisco

Attached Files

peteroznewman posted this 02 March 2019

The B file has the last two joints of 8 faces to 1 vertex. This is wrong. You should have 1 face near the vertex for each joint. This is the reason why the finger is stiff.  That one joint is connecting all the cable holes together into one rigid spiderweb.

You can get rid of the warning message by suppressing the pin body that is fixed and replacing it with a Fixed Support on the holes where the pin was.

 You need to add the contacts that prevent the finger from bending backward.

peteroznewman posted this 03 March 2019

It seems there are two cases that you want to examine the stress in the assembly.

1. Back-bending force on the fingertip with straight finger.  In this case, the cables contribute very little stress, it is the contact that prevents the finger from bending backwards. This will solve very easily and the stress can be very high for a moderate force on the fingertip.

2. Fingertip supported by remote displacement (straight finger). In this case, the fingertip is prevented from curling by the remote displacement, that simulates contact with a rigid surface. The cable tension develops the stress in the assembly. This will solve very easily.

The zero resistance curling of the finger by changing the stretch of the cables is almost impossible to solve using Static Structural, but this is also not an important analysis to compute as there are no high stresses in this case.

Francisco Guerra posted this 04 March 2019

The B file has the last two joints of 8 faces to 1 vertex. This is wrong. You should have 1 face near the vertex for each joint. This is the reason why the finger is stiff.  That one joint is connecting all the cable holes together into one rigid spiderweb.

You can get rid of the warning message by suppressing the pin body that is fixed and replacing it with a Fixed Support on the holes where the pin was.

 You need to add the contacts that prevent the finger from bending backward.

It seems didn't explain myself very well, but the technical question was why I should have 1 face with 1 vertex for each joint and you answered me in your post , thx. 

Following your recommendation, I tried to get rid of the warning message by suppressing the body pin, but didn't know with which other piece or how to link the revolute joint of the 3 phalanx, because it was linked with the body pin that I suppressed

 

Francisco Guerra posted this 04 March 2019

It seems there are two cases that you want to examine the stress in the assembly.

1. Back-bending force on the fingertip with straight finger.  In this case, the cables contribute very little stress, it is the contact that prevents the finger from bending backwards. This will solve very easily and the stress can be very high for a moderate force on the fingertip.

2. Fingertip supported by remote displacement (straight finger). In this case, the fingertip is prevented from curling by the remote displacement, that simulates contact with a rigid surface. The cable tension develops the stress in the assembly. This will solve very easily.

The zero resistance curling of the finger by changing the stretch of the cables is almost impossible to solve using Static Structural, but this is also not an important analysis to compute as there are no high stresses in this case.

As you said, I'm interested in the stress in the assembly with straight finger due to the forces (or displacement) in the cables, with both displacements simultaneously like in the A file, so that is solved (independently of the warning message).

Now I'm trying to simulate displacements independently to get the stress in the assembly, first a simulation only whit the top cable (back bending force resulting in a slight upward curvature) and then another simulation only with the bottom cable (back bending force resulting in a downward curvature).

I'm working over the A file (simulating top cable only) suppressing all the contacts and joins related to the bottom cable displacement in order to have the stress due to the displacement of 7mm in the top cable, but after many attemps the simulation doesn't converge... any recommendation Peter about what I'm doing wrong?

Thank you again, best regards,

Francisco

Attached Files

Close