I have a simple roller. I use the revolute joints and try rotate the roller and observe the deformation. What is reason I get such large deformation? I expect deformation very very minimum. Please help how can I solve the problem. I also have attached the simulation file herewith.
rotation in angle
I have a few comments.
1) Why are you rotating the body? The only force on it is Gravity. Once you see how the roller sags due to gravity, it will sag that way at any angle of the roller, since the roller is symmetric.
Even if the roller was not symmetric, it is much more efficient to rotate gravity around the roller than rotating the roller mesh. You can't do that with Standard Earth Gravity, but you can do that with Acceleration.
2) Two revolute joints over-constrain the roller. A revolute joint takes the length of that shaft and prevents any bending or tilting of the shaft. If you have a single row of ball bearings at one end, that tends to allow bending and tilting of the shaft. You can change the joint type from Revolute to General and free up all Rotations. You have to add one more constraint, a Remote Displacement to hold the rotation fixed or displaced.
3) The deformation is exactly what I expected to see. The distance a node on the surface at a radius of 100 mm travels from its start position to its end position after 60 degrees of rotation is exactly 100 mm.
1) My idea was to check the deflection of the roller due to it's own weight with different rotational speed and to compare the deformation with the static case(without rotation). Since I couldn't give rotational velocity on that revolute joint in the static structural system, i tried providing the angle for rotation. I assume that the deformation should stay something simlar(on both static and rotating state) unless the rotational velocity is too high.
(2&3) It's clear for me. And thank you!
Look under the Inertial load category on the Environment toolbar and you will find Rotational Velocity. That is what you were looking for.
Did you delete your question on Nip Mechanics? I wrote a comment on that, but now the discussion is gone. Here is my comment anyway.
What is the construction of the roller, is it a hollow metal drum? Is there a hyperelastic material covering on the surface of the roller? If the answer to both questions is yes, then the pressure is higher at the edges than the center. That can cause problems because the speed of the media increases with nip pressure. If the edges are moving faster than the center, that can lead to wrinkles forming in the web.
Thank you for the information. I didn't see the comment because may be my page wasn't updated. So, I just wanted to post again with clarification and pictures so I deleted last post. The below picture shows how my mechanism looks. The roller geometry is similar to drum and the material is general steel without any covering. And i am concerned about the orientation of the Veneer sheets leaving the nip roller, which is expected to be straight always but it is turning in reality. Mostly I would like to see how the bending of the long roller or slippage in nip is related with the turning of the sheet using simulation.
What is the gap between the rollers and what is the thickness of the sheet?
Hello gap between the rollers is around 3 mm when the sheet thickness is 4 mm and the speed of the roller is around 40 rpm(around 4 rad/s) and i forget to mention that the upper roller is free to move in the vertical direction. In order to simulate whole mechanism, I want to simplify the mechanism without gears providing equal velocity for each roller. I would like to just rotate both the rollers with some gap and later add the web material(Veener sheet) and do contact simulation. But First of all I would like to just simulate one of the roller.
*) I am trying to simulate one of the roller as shown in mechanism picture in the post above. I wanted to simulate the roller rotating with velocity 4 rad/s while it's bending(deforming) due to it's own weight(gravity), like which happens in reality. And I tried to follow as your instruction in your earlier post. Looks like I have problems with constraints and the result is weird, could you please have a look? Or any open suggestions are welcomed as well.
I also tried to simulate nip roller accordingly and the simulation couldn't be solved. I have attached file here with this message. For temporary time, I am using nonlinear Aluminum material as a Veener sheet. It would be nice to get some help, what is wrong with those constraints according to my mechanism drawings. I have provided each roller rotation of 4 rad/s but in opposite direction in order to pull the sheet into the nip.
Do you already know the physics of why the sheet skews (rotates in the plane) as it passes through the nip, or are you trying to learn that in the simulation?
Comments on the Full model in Static Structural.
1. change the roller drum from a solid body to sheet bodies in DM by using the Midsurface feature so you can mesh with shell elements. You can represent the solid shafts at each end with a line body and assign it a circular cross-section to mesh with beam elements.
2. the Veener sheet must have > 3 elements through the thickness, and maybe as many as 12 elements to capture the permanent deformation due to the plasticity in the material model.
3. If you are only studying symmetric configurations, single sheet in center or two sheets symmetrically offset from the ends, you can cut your whole model in half at the center of the width of the roller.
4. Add a mesh control to put 180 elements around the drum circumference. You can't have large elements like you have now. Make similarly sized elements on the Veneer.
5. Put the veneer into the nip so some material sticks out the other side.
6. Ignore the centripetal forces on the drum and delete the two Rotational Velocity BCs. Those forces are very small compared with the forces needed to deform the Veneer.
7. Ignore gravity forces on the drum as that force is very small compared with the force needed to deform the Veneer.
For a one roller simulation, you can put a plane through the center of the veneer and use symmetry. That is a good first model.
a) I don't know yet the physics behind why the sheet skew so, I am trying to find the reason why it skews using simulation. And, I suspect that deformation cause by roller's own weight may be the reason for the Veneer skewing on the plane, Since roller is quite long about 6 meters. And also when I perform static analysis placing one roller just over other, it shows upper roller deform less than the lower one making uneven gap between the rollers.
In real process, two veneers goes inside the nip just as shown in the picture and also skews just similar to what it is shown in picture, i.e mostly skews outwards from center line of the roller.
Is the purpose of the rollers to plastically deform the veneers to a thinner state than they went in? Or is it just to transport them?
The main purpose is the transportation and it's inside the dryer with the temperature around 200 degree Celsius.
What is the nip force?
If you are just transporting, then you wouldn't expect to exceed the yield strength of the veneer would you?
Hello peter,
I tried my analysis as per your instructions(mostly). For now i have ignored the four end rods. Nip isn't pulling material into it. I assume mesh are better now as well. What can I do to improve the sheet material drawing inside the nip? I have only used small sheet to reduce the time for solution. I have attached file as well as few pictures from my simulation.
I don't know the nip force. Even though the main function of the nip is transportation, the veneer sheet are compressed as well. The nip load is all generated by the roller's own weight, as the upper roller is free to move in vertical direction and pressing the sheet. And you are right, it shouldn't exceed the the yield strength of the veneer.
And I have one more question, how is it possible to create the veneer material in Ansys, or does ansys already have some built-in material for wood or veneer sheet?
So the nip force is the weight of the top roller. How much does it weigh?
You need many more elements around the diameter, from #4 above, use 180 elements around the drum circumference.
Also put the veneer more through the nip so it sticks out the other side.
When you said you used Aluminum, I thought that was the actual material. Is this material a single veneer of wood? If so which way does the wood grain direction go?
What is the humidity of the environment? Has the wood been exposed to water prior to this roller?
a) You are right nip force is the weight of the top roller which has a mass around 60 kg and upper roller gets torque from lower by two spur gear(gear ration 1:1) mating mechanism.
b) I have added more element but i am out of memory, I will have to find next computer with more memory or shorten the roller for simulation purpose.
c) If the gap between roller is 3 mm and veneer sheet is 4 mm thick, please let me know how can I define the contact between veneer surface and roller surface if I let all the veneer through nip. I mean veneer surface will intersect rollers surface.
d) Yes, this material is single veneer of wood and wood grain direction goes perpendicular to the width( 6 meter) of the roller.
e) In my case, the material is soft wood, for example pine is good.
f) I exactly do not know the humidity, so I can let you know later. And before peeling yes, wood are soften by sprinkling water. But after peeling, I assume Veneer sheets remain for some days in stack and later it is inserted into dryers. (I can add more info in my next reply, if i find about this description)
b) Use symmetry to cut the model in half. Did you midsurface the roller drum? What do you mean you are out of memory?
c) move the roller to be 4 mm apart, tangent to the veneer, or let the contact lift the roller to the 4 mm point in the first step.
e) you can look up properties of Pine from the link on the discussion from last year.
B) Yeah I have cut the model in half and also used midsurface the roller drum. For example if I have 8 gb of ram, the ram is fully loaded and the simulation stops itself without warning. Or sometimes it also give the waring.
-I reduced the number of element and perform the simulation. It doesn't pull the material into nip and looks like it's sliding just at same position. And I don't get any deformation on the veneer sheet. What could make this happen? I have attached force convergent solution diagram with this message and it slow that force is converged at very minimum value(around 4e-5).
Is that I have to define contact between the roller shell surface(midsurface) to the sheet material in different way ?
How did you define the contact? Show a screen shot of the details.
The screen shot showing the details of both the frictional contact.
What does the contact tool show?
Please show the mesh near the nip.
How are you applying a nip force?
Try a two-step solution, in step 1, just let the nip force ramp on while the rotation is set to zero, then in step 2, apply some rotation.
Hello Peter!
I though that my model was quite big that I had many elements and nodes. Because of it, it took quite long time either to get the solution or to get error messages. So now I am starting with so simple model and with shorter width of the roller. Simulation is going good so far even though it has some pivot error for now.
I have a question about the material. My material for the veneer sheet is pine, which is a soft wood. I found the material properties for sugar maple in your earlier discussion. Will it be fine, if I find all the material properties value like for example sugar maple as shown in the picture below. I think if I am dealing with temperature as I move on, I assume I need some temperature properties for the pine as well? If I need to add any more material properties for my case, it would be nice to know.
Sugar Maple is a hardwood, so would have different properties to pine, which you correctly state is a soft wood.
Hello again,
Is it possible to model slippage in Ansys? The veneer sheet passing through the nip has a higher chance of slippage because of the slight difference in surface velocity of the roller in our case. It was also found that nip-pressure was higher towards the end due to the deflection of the roller.
I read some of the posts regarding slippage from you. And I think that it's not at least possible to simulate slippage in the static structural mode because the moment it starts to slip, the solver gives the error and it stops. Could you please give some hints for slippage simulation, if it is possible in Ansys regarding the case?
I have seen 3D finite element models that simulate the transport of a sheet of paper between elastomer covered rollers where the paper skews as it is transported due to differential nip pressure from the paper being on one side of the centerline of the rollers.
The paper, or wood in your case, is wide enough so that one part can be sticking while another part is slipping. This allows a static structural model to make progress.
Thank you once again for the reply.
a) Are there any tools or technique to see either the surface is slipping or not? For example, contact tools at the result section have options to observe either the surfaces are sliding or sticking but not slipping?
b) Is there any way, I can make a connection like shown in the picture. There are a slot and a shaft. I want the free rotation of the shaft, as well as the free movement of the shaft in Vertical direction. I have tried using general joints but it doesn't allow me to rotate and if I use the revolute joint, it will fix the movement in a vertical direction. Is there any other combination(joints and contacts) we can use to make such connections?
The contact tool allows you to plot the contact status
Status. Status codes include:
0 - open and not near contact.
1 - open but near contact.
2 - closed and sliding.
3 - closed and sticking.
There is also sliding distance.
Sliding Distance - available only for evaluating contact conditions after solution. The total sliding distance (SLIDE) is the amplitude of total accumulated slip increments (a geometrical measurement) when the contact status is sticking or sliding (STAT = 2, 3). It contains contributions from the elastic slip and the frictional slip. Elastic slip due to sticking represents the reversible tangential motion from the point of zero tangential stresses. Ideally, the equivalent elastic slip does not exceed the user-defined absolute limit. The higher the tangent stiffness, the smaller the resulting elastic slip. The pair-based elastic slip can be monitored using the Contact Result Tracker.
You have two bodies, a fixed body with a slot feature and a second body that is a roller. Add a third body in the slot at the roller end. Put a translational joint between the slot body and the third body, and put a revolute joint between the third body and the roller. Now you have a roller that can translate up and down. However, this combination doesn't allow the roller to tilt away from horizontal without bending either the roller or the slot. You didn't mention if you want this freedom or not. If you replace the revolute with a spherical joint, now the roller is free to tilt in two directions as well as rotate.
Thank you for your reply.
Yeah, I forget to mention that I wanted the shaft which is connected to the third body tilt as well. So, now, I used spherical joint so that shaft can tilt on the third body.
But now I would like to give the rotation to the shaft without affecting the tilt(spherical constraints), which means the center of rotation should change as shaft deforms and also rotate at same time. How can I do so? I couldn't give rotation using a spherical joint. If I use the body to ground revolute joint at the end edge of the shaft, that will constraints rotation/tilt which is created by spherical joint before.
In real design, the shaft is connected to the third body using plain bearing or bushing, so I am trying to get close to that constraint situation.
I have added the picture, how my design looks with a slot and spherical joints.
Mechanical has Bearings that are appropriate for small deformations. You get to define three spring rates of the shaft to ground, horizontal, vertical and 45 degrees.
Try using a General joint to ground that only constrains rotation about the shaft axis and use a Joint Load to drive rotation.
peteroznewman
245
rwoolhou
96
abenhadj
79
tsiriaks
61
Aniket
36
madelpa
21
Autonewbie
16
Supreethm
12
Alex1EDP
11
vsmlingam
9
