Displacement Even Without the applied load 1

[Svillefan08]

I'm currently designing a device used to grip medical needles. IE one end of a shaft is pull through a scissoring action and as a result two faces come together to grip the needle that is between them.

I am trying to run an analysis on the assembly to look at stresses as the shaft is pulled and the faces are pressed together (no needle). The faces are initially coincident.

However, I am having the problem that, despite pulling on the shaft in the negative Y direction, there is movement in the positive direction, causing the faces to separate, and ruining the analysis. To try and locate the problem, I removed the applied load on the shaft, and re-ran the calculation. Despite there being no load, there is still movement of the shaft in the positive Y direction, causing the faces to open. Does Anyone know what would cause this problem of displacement without an applied load?

 

[franc11HD]

Did you put a contact connection between the faces? Because if initially the geometry of the faces are slightly overlapping, it creates an initial displacement to account for that overlap.

But honestly, with applied loads, there should not be any displacement.

Are you sure you are converging? Is you model constraints in all 6 DOF? Sometimes, when you get a rigid body motion (lack of constraints) Catia solves while telling you that some DOF are not fully constraints. Then you are able to see the displacement, but not the stresses. What is the value of the displacement.?

 

[Svillefan08]

Before running the computation it give me the warning that rotation constraints are not taken into effect due to it being a 3d model. Then after computation is warns me that there is a singularity in the translation that may be due to improper constraints.

The scale factor for displacement deceived me, and I thought the translation was what would be expected for opening the faces, but it is actually an extremely large displace. Orders of magnitude larger than expected.

As far as I can tell though, there is every necessary constraint though. Most items are rigidly connected where Bolts or other connections would make them behave as so.

The only unusual connection I have is at 3 locations where parts need to be able to rotate about a pin connecting the parts through holes in each part. This was done as a rigid connection with the Rotation that was desired unchecked.

Otherwise the model is clamped on one end where it would be supported by a device that it is connected to. Images included to help with visualization. Had difficulty attaching so here are addresses:

http://files.engineering.com/getfil...-47b4-a6a7-c45e00616459&file=Gripper_Full.PNG

http://files.engineering.com/getfil...490a-b0ef-2dd1e29574c7&file=Gripper_Inner.PNG

 

[franc11HD]

Definitely, something is not constrained correctly. One thing you can do is lookat the displacement. Put a scale factor of 0.00000001, until nothing seems to have moved. Right Click on the result (on the screen)select vector components to show each displacement vector of nodes. Usually it helps visualizing what is moving. Then increase the scale factor until you see the part(s) moving. You can play a video of the displacement as well, itcan help.

Then you shouldbe able to see what constraint is missing.

It's hard just bylooking at your pictures to tell what is missing and what meshed in all that.

If you could send pictures showing all the constraits applied to the model and the mesh, maybe I could help you debug this.

Another trick, is to clamp all the parts there is in the model. The model should run. Remove one clamp after the other to see when rigid body motion occur and whic part causes that.

 

[Svillefan08]

Yes, I would greatly appreciate the help. Attached are images of the entire piece and all of the connections in it, along with the resultant vector field of the failed analysis, on a scaled down factor.

5 pics explaining connections:

http://files.engineering.com/getfil...2-4643-bb31-40573d873244&file=Inner_Pic_1.bmp

http://files.engineering.com/getfil...2-4209-8ed5-b6ebb454c17d&file=Inner_Pic_2.bmp

http://files.engineering.com/getfil...a-4124-9771-b8e4cfe33c2a&file=Outer_Pic_1.bmp

http://files.engineering.com/getfil...9-4972-9bd0-965fa27d95ba&file=Outer_Pic_2.bmp

http://files.engineering.com/getfil...-ce0c-4c62-8f3a-1d80a3e56bb3&file=End_pic.bmp

2 Images of Vector Field:

http://files.engineering.com/getfil...610-fbab01c27511&file=Shaft_Displacements.bmp

http://files.engineering.com/getfil...-906510034d41&file=Scissor_Discplacements.bmp

Judging by what you have said, I imagine the problem is probably the fact that the piece isn't constrained in any way to stop it from opening. I did not create this restrain because I could not find a way to constrain it other than by rigidly connection the two faces of the scissors. I did not particularly want to do this because I felt it would probably change the results. I did not think this would be a computational problem because the force I was applying was not causing it to open. The force I am applying causes the scissor to close (It begins in contact so there is no actual "closing" but it should apply pressure between the two faces)

The end goal of this analysis is to see if the application of forces to close the clamp causes significant bending moment in the "Force Sensor" face that connects it to the connector. This is either face that has the red rigid connection.

 

[franc11HD]

Seeing the picture, it is a fairly complex mechanism. One thing you hsould do when dealing with such assembly is "are all DOF of the mechanism is constrained? This means without the force, is there anyway, wany parts can move in any of the 6 directions (3 translations, 3 rotations)

This is a static analysis, which means it is an frozen instant in time. No movement are allowed per say. For example, in the second result pricture, you see that the scissor rotates about 1. Of course it does. The rigid connection allows that rotation (as you explained) but what in real life prevents taht rotation? No other connections prevents it. So that is why you have a rigid body motion of the scissor sbout that rotation axis.

Same thing for all the inner shaft portion. With the sliders, you prevent any translations, but nothing prevents this whole assembly to rotate around the inner shaft axis. I Think that is what we see on your first result picture. For that inner shaft, just add to the outer face (where the load is applied) a constraint in rotation about the axis. Should solve part of it. For the scissor, I would actually fix the scissor aprt with that two hole "squarish" thinf together (lets say on the two surfaces that are in contact. This will prevent the scissor to rotate freely about 1. But everyting could still rotate around 2. So you would need to fix the hole 1 in translation (only). So by pulling on 2, the only thing the mechanism could do is to rotate around 1. This should give you the movement you want.

You need to understand that this is not a dynamic body motion analysis you are performing, everything needs to be fixed in someway to get stresses. For example, a straigth bar is pulled. Stresses only can occur if an equalt load is applied at the other end (or constrained in that diection).

You need to go parts by parts and look at any DOF and ask yourself is this part can move freely. If not because constraint by another part, than go to that other part and ask the same question. For example, you can attach two parts together, but as long as those two parts are not fixed in the space, they will still move together, but all around the place.

AT last, when everything is constrained, then you need to ask yourself if that model and the way it is constrained really repesent the reality or what you want to try to simulate.

One other thing, I am not sure why is the purpose of the outershaft. It doesnot seem to be connected to the inner shaft in any way. Therefore, no forces are transmitted on it. So it is useless in your analysis. But you could use it to constrainthe inner shaft (instead of applying a slider to the inner shaft, you could create a slider connection between the inner and outer shaft.

Anyway, it is hard to really help without having it in front of me a playing some time with it. But hope this helps a little bit.