Analysis of Robotic Finger
-
-
-
.png)
-
-
-
-
I TRIED DOING THE SIMULATION WITH ONLY 2 JOINTS THAT IS MAKE ONLY 1 MOTION RATHER THAN COMPLETE FINGER TO MOVE AND I SUPRESSED OTHER CONTACTS AND BODIES TO DO THIS. CAN YOU ONCE CHECK MY ARCHIVE FILE ATTACHED IN ABOVE LINK
-
-
-
What is the purpose of this simulation? What is the output you want the simulation to generate?
Have a closer look at the example cable driven joint I provided. Notice that beam elements were used to mesh line bodies that represent the wire. That is much better than what is in your model which has the wire meshed as solid bodies. This is to be avoided because it creates a model that takes a very long time to solve.
-
-
1 kg is a mass. You mean supporting a 1 kg mass with the finger horizontal. Where exactly on the fingertip is this 1 kg mass? Nearer to the joint or the tip or in the middle of the fingertip pad?
You want to know the tension in the wire (thread) when this 1 kg mass is being supported.
Please create a cross-section of the links in the YZ plane through the center of the wire in the X direction. Show where the wire touches any part and what locates each end of the wire: the end fastened to the fingertip and the end where the wire is pulled.
It may be easier to converge if you replace the wire with several spring elements. At the points where the wire bends around a corner, a dummy body will be used to represent that corner. The spring on each side of the corner is attached to the dummy body which will have a revolute joint to the center of the corner radius. The revolute joint can measure the normal force and provide a coefficient of friction at the appropriate radius. This will be much more computationally efficient than trying to get the wire to make frictional contact with the corner.
Instead of using an actual mass and gravity on the fingertip, use a remote displacement instead and just fix Z = 0 leaving all others Free. Then you can pull on the end of the last spring to tension the “wire”. When the reaction force at the fingertip reaches 9.81 N, you will know that the fingertip is supporting a 1 kg mass.
-
Here is a cross-section. The link design has a rotation stop prevent rotating each link back past this extended configuration. The finger can only curl up from this point. In this configuration, a large mass can be supported without any tension in the wire. I assume you want to know the tension needed to curl the fingertip up, is that correct? I don't see a wire to tension to do that. I see a light tan wire that when tensioned could curl the middle segment of the finger up. I also see a wire that could curl the first segment of the finger from the palm. Please clarify which segment of the finger you hope to move to lift the 1 kg mass.
-
Now I can see the wire to curl the fingertip.
-
-
You have drawn a bent wire, and that is the shape that has zero stress before load is applied.
If you were to have a fixed support on the fingertip and simply pull the right end of the green wire in the +Y direction to straighten the wire with no contact with anything else, you would generate bending stress all over the length because you are straightening the wire. The natural shape of the wire is straight. That is the shape that should have zero stress under zero load.
To obtain the correct bending stress in parts that change shape when they are installed in a mechanism, draw the part in the shape that has zero stress, then assemble the part into the mechansim. This is explained fully in this discussion.
For components like wires that have very low bending stiffness but very high axial stiffness, or bicycle chains that have many short links with joints, you can draw the parts in the assembled shape. The problem in your model is your solid wire does not have a very low bending stiffness. It has the same stiffness in every direction. That is why you won't get accurate stress in the wire using a mesh of solid elements with an isotropic linear elastic material model.
-
-
Rohith, I’m not sure you understood my point about using solid elements, linear elastic materials and drawing wire bent to conform to the path through the mechanism. The bends you draw in the wire remain in the wire as it is pulled around a roller. I created an example to show the behavior of the method you are using. It consists of a wire that has a 10 N downward (-Y) force on the bottom end of the wire that is drawn around a frictionless roller. The other end of the wire is pulled 5 mm along the +X direction. Contact is frictionless between the wire and the roller.
Here is the deformed shape at the end of the simulation.
This model used solid elements, but you would get the same result with beam elements. I hope this makes my point clearly.
You could use the line bodies that allowed you to mesh with beam elements, but mesh with LINK180 elements instead, which have no rotational degrees of freedom and so you can draw them bent and they will straighten just like a bicycle chain straightens when the sprocket turns.
-
-
Here is the line body meshed with Link180 elements at the start of the simulation:
Here is the simulation after pulling the end 5 mm.
Here is a link to the the ANSYS 2023R1 archive without results.
-
-
-
-
Hi peter i changed the strings to beam elements and when doing so the beam are not connected properly even though there is no gap and when im trying to connect it the shape of string is disturbing and even trying with share topology feature the other links are getting joined and making a 1 body making difficult to give joint and contacts how to solve this -
-
I HAVE CONVERTED THE SOLID ELEMENT TO BEAM ELEMENT BUT WIRE IS PENETRATING INTO THE BODY WHILE PULLING AT THE END HOW TO SOLVE IT?
-
The nodes at the center of the sting do not penetrate the edges of the hole. I suggest you offset the hole surface by the radius of the string then the centerline of the string will be in the correct position when the nodes contact the offset surface. In the first image below, the surface has been offset to reach the nodes at the center of the string. If you turn off the thickness on the beams and shells, you can see that the nodes touch the surface.
An alternative is to use a setting on the Contact Definition: Add Offset, No Ramping to the Interface Treatement under the Geometric Modification of the Frictionless Contact definition. In the image below, with the thickness turned on, it seems like the string sits on the roller. But in the next image, you can see that the nodes are offset from the surface.
-
Solution is not converging after few iterations
-
-
-
Reread my reply earlier in this discussion when I said a Beam model will give the same result as a Solid model of the string when pulled over a roller.
If you study my model, under the Geometry branch, click on the Beam (Circle) object and in the Details window, you will see Model Type where you can change a Beam to a Link/Truss element.
I shall warn you that since you found it difficult to obtain convergence with Beam elements, you will find it 10 times more difficult to obtain convergence with Link elements. The reason is the shape of a chain is unstable unless it is under tension. Extra effort is required to put the Links under tension before any movement can occur. A string of beam elements is stable on its own if you hold one end fixed.
Reread the paragraph above beginning with "It may be easier to converge if..." that I wrote in the March 21, 7:28 am reply.
-
made changes as you said no result
-
-
-
Here is an example where the many Link elements have been replaced by 2 spring elements. The roller has become a rigid body with a revolute joint at the center. The ends of the spring are scoped to the rigid body. This kind of model is useful to evaluate the forces in the mechanism at a particular configuration. It is not as versatile to operate the mechanism through large angles of rotation of the joint, but it is easy to build and easily converges.
-
-
-
Hey peter just a small doubt i need to simulate small screw to rotate about its own axis and revolve around the central screw i tried by changing the positions of the joint but it didnt worked could you juat check my archive file once and suggest me changes required SCREW
-
-
HI PETER I CHANGED THE WIRES TO CABLE ELEMENT AND ATTACHED SPRINGS AT THE END TO MAKE IT LOADED WITH STIFFNESS VALUE OF 1 EVEN THOUGH IT IS NOT SOLVING WHEN THE INTERFERENCE TREATMENT WAS GIVEN WITH ADJUST TO TOUCH IT IS BEHAVING LIKE THIS AND WHEN I GAVE ADD OFFSECT NO RAMPING THE STRINGS ARE PENETRATING INSIDE THE BODY IM NOT GETTING ANY IDEA LIKE HOW TO SOLVE THIS COULD YOU JUST HELP ME IN THIS
-
-
-
In the archive, there is one wire, but two revolute joints. Tension on that one wire is going to affect both joints. This is unsuitable for the simplest example.
Keep the revolute in the top viewport and change the revolute in the bottom vewport to Fixed. One wire can only move the link up. There should be another wire that will move the link down. For now, we will just work with one wire.
-
-
Here are the results of a simple model using a spring to determine the tension in the wire when there is a 9.8 N (1 kg mass) on the next joint in the finger. You can see the wire has been replaced with a spring. The spring has a line of action that makes it tangent to the surface of the finger the wire would be tangent to if it were wrapped around that surface and anchored further to the right. The other end of the spring is tangent to the hole in the fixed part.
The unknown is the tension in the spring under this load. This simple model quickly calculates this value to be 64.7 N
The spring rate is a large number to prevent large movement of the link so the tip of the link only moves 0.12 mm.
-
-
Complex models are often assembled using a large number of simple components. I demonstrated how several simple components work.
The component using Link/Truss elements has the benefit of being able to wrap around surfaces and slide on corners but the drawback is they are very difficult to achieve convergence, which can become exponentially more difficult as you add a large number of them into a complex model.
The component using Spring elements has the benefit of very easy convergence and provides the most important information but has the drawback of missing some information which would have to be obtained by other means. However a model with lots of springs is not likely to have convergence problems.
If you really want to use a wire, you must be precise in constructing the wire so that it is drawn tangent to the surfaces it must slide on. Below is the cross-section of the wire. Note that it is not tanget to the surface of the finger and is not tangent to the hole in the fixed part.
The wire must be perfectly straight from one tangency point to the next. You can’t draw any curves unless the wire is in contact with a curved surface, and in that case, the curvature must match exactly. You can’t draw wiggly wire as shown below. The consequence of doing so is that convergence becomes impossible.
Below is an example of a straight wire that wraps on the surface of the link.
To construct the line on the surface of the link required a lot of geometry construction. First a 3D line from one point to another, then a plane on that 3D line, then split the surface on the top of the link with the plane then extract that curve which is an ellipse, then draw a line from the edge of the hole to the tangent point on the ellipse. That is a lot of work for just one section of one wire.
The nice thing about springs is they are straight lines between two points and even if the end points are not exactly at the tangency point, the solution will easily converge and you will get some useful information.
-
-
-
-
It's all about the geometry. If you can't construct two lines tangent to two circles, there are no settings that can fix bad geometry. Below is what good geometry looks like.
Below are the wires you had. Do you see my point about straight lines tangent to surfaces? You don't have that.
-
-
For the method of using springs instead of wires, I sliced off a piece of the body and colored it purple to act as a "roller". I will put a revolute joint between that cylinder and the adjacent part of the link. The springs will model the straight part of the wire. This allows the springs on each side of the roller to have the same tension. For the method of using wires, slicing off a piece is not necessary as the wire would slide on the surface of the boss in the link.
-
For the method of using springs instead of wires, I sliced off a piece of the body and colored it purple to act as a "roller". I will put a revolute joint between that cylinder and the adjacent part of the link. The springs will model the straight part of the wire. This allows the springs on each side of the roller to have the same tension. For the method of using wires, slicing off a piece is not necessary as the wire would slide on the surface of the boss in the link.
-
-
Below is the method of using springs. This is the one that easily converges and provides the tension in the wire for an applied load. The springs attach at the tangent points.
There is a tip load of 9.8 N. The Displacement is X=0 to support the tip because I cut the model in half. The Remote Displacement pulls on the spring to lift the finger tip.
Frictionless contact prevents middle link from back bending.
The spring probe shows the springs need 54.77 N of tension to lift the 9.8 N on the finger tip.
Here is the ANSYS 2023 R1 archive of the spring method. I understand you want to see the method of using wires, but that is much more difficult to converge. The wires needed to attempt the wire method are in the archive as suppressed bodies. You are welcome to try it. I don't recommend it for this model.
-
thanks peter but i want to solve with wires and want to know the contact stress and behaviour of wire at edges i the file the wires are suppressed but they are not assaigned with any contacts or loading conditions i cant understand how to give pre tensions and contact settings for those could you just solve with the wire which is passing through the edge which i find it more difficult even to assign the settings. i just want to understand the conditions you apply for link elements
-
-
i think it worked for this string but i cant be able to solve with the wire that is passing and bending over the edge how to solve it
-
when i was trying to pull the end of the wire that i have model mostly straignt and tangent to surface it is penetarting into the link and the contact status is closed in initial condiction what could be the reason for this kind of behaviour could you just check this once wire model
-
This new wire is not modeled as straight (see green arc) nor is it tangent to the sliding surfaces. Geometry defects like this make it impossible to converge.
I recommend the spring method to get an initial estimate of the tension in the wires needed to support a tip load.
-
I had drawn the wire in contact to the edge so that it will be in tangent to the surface even after doing that the wire is penetrating into the link
-
-
yes peter but my project includes the behaviour of the wire i need the contatct stress, tension which are from the wire model only and the one which i have mentioned above worked when i moved the center wire little down but as mentioned i not getting solution for wire which is passing through edge of the link when pulling from one end i have modeled the wire with mostly straight elements and it is tangent to the top link surface but i cant to able to obtain the solution i have attached the pictures of my contact settings and boundry conditions with the lin to archive file edge sliding
-
If you extrapolate the trend, you would predict that the lines will cross and the solution will converge, if only the solver would have kept iterating! Can you think of the place where you told it not to give up until 50 iterations? Why don't you change the number from 50 to 100 and see what happens?
I initially did some work on the wire that goes off at an angle to the side while wrapping around the arc of that link. It seemed to me that the wire is on the verge of sliding off the arc and ending up at the side of the link instead of on top. That kind of sudden change in contact status is toxic to convergence. This is not a good design. The link should be wider at the base so there is no chance that the wire will slide off the edge. Bad designs are harder to simulate than good designs.
To address the need to know the contact stress of the part the wire slides on, I would build a dedicated model just for that. It would be a very simple model like the ones I provided above. I would make it a parametric model that will create any of the wire contacts in the assembly. The parametric inputs are the bend radius, the wrap angle and the tension. Using the Parameter set capabilities of Ansys Workbench, you can copy/paste a spreadsheet with as many rows of inputs as you like, then click the Update All Design Points and Ansys will automatically build each of those models and solve them to report the contact stress. The system model of the entire finger (using springs) computes the wire tension values for any load in any configuration. The system model can also be a parametric model to assemble the links in all configurations of interest. By separating the analysis into two models, each one converges easily. This is a great approach that is a widely used by analysts in many fields.
-
Hey Peter, I tried to make the wire model as tangent as possible to the edge where it gets wrapped. The solution converged until 1 sec, in which the wire glided along the edge with wrapping but after that, the solution is not converging and terminated could you find the reason for it edge
-
The reason you request Newton-Raphson Residual Force plots is to find out where the solver is having trouble converging on a force equilibrium. As you can see below, it is where the wire is bending over a sharp edge.
It was a bad idea to have the wire bend over a sharp edge in order to reach down to the dowel pin in the FEM. It would be a good idea to end the wire at that corner so that it never has to bend over that edge.
If you really want the wire bending over that edge, then you should put a blend radius on that edge but I would not do that. Just terminate the wire at the corner.
-
This is the result of removing the last segment of wire and redefining the Fixed Joint to holding the next vertex. The other change was to set the Initial and Minimum Substeps to 100 and the Maximum Substeps to 1000.
Notice that the solver can’t get started, and has bisection before the first converged substep after 5 iterations with this warning:
EQUIL ITER 5 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= -0.2124
*** WARNING *** CP = 7.641 TIME= 21:22:20
Contact element 85693 (real ID 10) status changes abruptly from contact
(with target element 86405) -> no-contact.Below is the displacement of the first converged substep. Notice that the wire has left the hole at the very first substep
The Displacement condition shown below leaves the end of the wire Free in two directions. This is a bad idea. The wire is being pulled in a straight line along that local Y axis. Why not fix those two directions at 0, that would be a more stable configuration.
Making this suggested change results in the wire staying in the hole.
-
Notice that your contact definition is only on the exit from the hole. There is no contact for the entrance to the hole, which is only required as the angle of the wire changes.
-
-
-
-
-
Applied all the changes you suggested but no improvement
-
- The topic ‘Analysis of Robotic Finger’ is closed to new replies.
You are navigating away from the AIS Discovery experience