Learning Forum

[Rameez_ul_Haq]

Hello there. As it can be be seen that a fixed joint has an option of selecting beam behavior for both reference and mobile surfaces. How does beam behavior differs from rigid and deformable behavior?nSecondly, there is an option of setting a connection as beam itself, so what bascially is the difference between this and the one mentioned in the previous paragraph?n

[peteroznewman]

JOINT CONNECTIONnA joint has a single coordinate system. All the forces and moments pass through the origin of that coordinate system. You should only select Mobile and Reference geometry that is close to the coordinate system origin. If some geometry is very far from the coordinate system, huge moments can be created which can affect solution accuracy.nA joint creates two remote points at the coordinate system origin. The fixed joint rigidly connects the two remote points. Other kinds of joints allow motion in one or more DOF.nThe Behavior of each side can be selected as Rigid, Deformable or Beam. If Beam is selected, beam elements are created between the Remote Point and each node of the selected geometry. A Rigid selection adds infinite stiffness to the selected geometry, a Deformable selection adds no stiffness to the selected geometry, while a Beam selection add some stiffness to the selected geometry. The amount of stiffness added depends on the Beam length, diameter and material.nBEAM CONNECTIONnThe Beam Connection automates the process of putting a beam element between the Mobile and Reference selections. The benefit of the beam is that forces and moments are transmitted by the beam element, which has two end points, in contrast to the single origin. This avoids the potential accuracy problem of a fixed joint where the two sides are far from each other.nThe Beam Connection adds the flexibility of a beam between the Mobile and Reference sides, due to the length of the beam and the selected diameter and material.n

[Rameez_ul_Haq]

Promoting a joint to remote points and then applying the necessary constraint equations to the two remote points and then suppressing the joint; will it transfer the same and equal forces and moments from one remote point to another, as it was doing in the joint case? Will the two geometries which were linked through the remote points and constraint equations behave in the same manner as they were doing the joint case?n

[peteroznewman]

The Mechanical User Interface provides meaningful names to things, such as a Joint. When you click Solve, code is written to a text file for the solver. The code written for a Joint is just multipoint constraint equations.nIf you suppress the joint and write constraint equations correctly, you will end up with the same code that the Joint would have written for you, but the Joint code is always correct and you might make a mistake writing constraint equations manually.nSo yes, the constraint equations will transfer the same forces and moments as the joint and the geometry will behave the same because behind the user interface, the same code would be written for the solver to use.n

[Rameez_ul_Haq]

Thank you for your clarification, Sir.nA guidance from you on this issue would be alot appreciated. For example, I want to link two remote points at distinct locations using constraint equations such that it imitates a revolute joint. However, I donot want the scoped geometries to have any transfer of forces or moments between them since they are located at two distinct far away locations. Is it possible to happen? Is it possible for us to let the solver know to create the same nodes links (or whatever the link solver creates) between the two geometries such that no transfer of force/moment occurs between them? Or will the remote points linked to each other using constraint equations will always have a transfer of forces and moments between them? n

[Rameez_ul_Haq]

And also, will switching the mobile and reference surfaces for a joint connection affect my solution and results? I know that the solving time will be affected which is dependable on the mobile (or in other words 'slave') face, but for some analysis i have already conducted, I see no change in the stresses and displacements within the joint connection, only the force and moment results is reversed. Is this phenomenon true always, for all the structures? Can we say the same thing for the reference and mobile surfaces when a contact (like bonded, no separation, friction etc) is made between them?n

[peteroznewman]

For a fixed joint, there is no difference when switching mobile and reference except for the sign on all the forces and moments in the results. Joints that have a DOF free, such as a Revolute, can have an applied Joint Load. If that load is a rotation of 10 degrees, when you flip mobile and reference, the joint will turn in the opposite direction.nI don't understand your 7:10 AM question. It would be easier to answer if you insert an image to show a concrete example. I can give you a gear pair example. Take a pair of spur gears of equal pitch diameter. We know that as one shaft rotates by 10 degrees, the other shaft will rotate by -10 degrees. If the stress in the gear teeth are not an area of concert, but something elsewhere on the shaft is the area of concern, you could suppress the gears and insert a remote point on each shaft where the center of the gear used to be. You could write a constraint equation that set the axial rotation DOF of the remote point on each shaft to be equal in magnitude but opposite in sign. This CE represents the kinematics of the gears that have been removed. This is a highly efficient way to get that motion compared with meshing the gears and using contact on the teeth to get the same kinematics. The constraint equation will result in a moment on each remote point to enforce the constraint equation during the solution process.nYou could have one remote point scoped to nearby geometry and far away, have another remote point scoped to nearby geometry. You could Probe the resulting deformation of both remote points and know the motion of each point without imposing any constraints on their motion. In that case, no forces or moments are going into the remote points, they are only there for output. The remote point can be deformable if you don't want to add any stiffness ,but just measure the average motion of the geometry. n

[Rameez_ul_Haq]

Sir I understand what you are saying. nPlease consider the following image.n3 solid separate beams (connected by bonding at their connecting ends) are represented as straight lines in above figure. Now if I apply the constrain equations between remote point 1 and remote point 2, such that their translation in the X axis, and rotation in Z axis is the same when force F is applied, then I want to know that is there going to be a transfer of forces and moments between the surfaces where remote point 1 and remote point 2 is applied? I am confused because we already know that be it be any joint, behaving in the similar manner as the constraint equations I applied, will transfer the forces and moments from one remote point (and hence from that one scoped face) to the other remote point (and hence to the other scoped face). But I donnot want this to happen here. I want only the bonding connection between the beams to transfer the forces and moments. How is it possible to do it?nIf you can kindly also clear out one more confusion which I already mentioned in my previous comment; does changing the mobile and reference faces in contact such as bonding will affect by solution i.e. stress and displacement results overall or no? I know the contact stresses will change but what about the transfer of forces and moments from one surface to the other in bonding?n

[Rameez_ul_Haq]

THIS IS A SEPARATE CONCERNnDoes the ANSYS solver which creates a mathematical model to determine the reaction forces in joint connections based upon the input force, is dependent on the mesh size? If yes, then is it dependent on the global mesh size or local mesh size (around the vicinity of the joint) or both? I have changed the global mesh size and it was revealed that it is indeed dependent on it. Am I correct? Not sure about the local mesh size changes' affect. The change in displacement and stress results makes sense since they are dependendable on the mesh size, but how is the reaction force linked to it?n

[peteroznewman]

SEPARATE CONCERNnThe total force going through a joint is almost independent of the mesh size, unless you have grossly large elements. The stress on the elements scoped to each side of the joint is dependent on the local mesh size. Local mesh size can be affected by global mesh size, unless a mesh control was added near the joint. It is always a good idea to do a mesh convergence study to make sure that the results don't change significantly as the elements get smaller.nFRAME STRUCTUREnA structure in 3D space needs at least six ground constraints to have a static solution. You have only provided two. An example of six constraints for that structure is Rp1 has zero displacement for X,Y,Z and zero rotation about X and Y. That is called a pinned boundary condition, or a revolute joint. That is five constraints. The sixth constraint would be Rp2 has zero displacement in Y. That is called a roller support. Let's call that set of constraints Pinned-Roller. You can have more that six ground constraints. For example, both Rp1 and Rp2 could be fixed in all six DOF. That would be a total of 12 constraints. Let's call that set of constraints Fixed-Fixed. The deformation at the force application point would be smaller with 12 constraints (Fixed-Fixed) than the deformation with just 6 constraints (Pinned-Roller) because the extra constraints are adding stiffness to the structure.nFor the Pinned-Roller support, the applied force on top causes Rp2 to deform along the X axis. Let's say the applied force at the top results in exactly 2 units of deformation of Rp2 along X.nI suppose you could remove the X=0 displacement constraint from Rp1 and replace that with a Constraint Equation where the X displacement of Rp1 is equal and opposite to the X displacement of Rp2. Now the applied force at the top results in Rp1 deforming -1 unit along X and Rp2 deforming by +1 unit along X. The total deformation of the structure is the same 2 units between Rp1 and Rp2 but the fixed point is no longer Rp1, it is now a point halfway between them.n

[Rameez_ul_Haq]

Sir, your last paragraph clues that you understood my point of view. However, please have a look at my previous comment where I re-mentioned the conclusion of our discussion, which said that linking two remote points using constraint equations will create a force and moment trasfer between them. Does this necessarily have to be matching the constraint equations of any joint to create this force and moment transfer, or always linking two remote points through constraint equations will result in a moment and force transfer between them. Also, I wasn't able to see in your answer if you have suggested that will the force and moment transfer occur between RM1 and RM2 linked through the constraint equations making their displacement along X direction to be equal?n''SEPARATE CONCERN''nSo what affects the force passing through a joint, assuming we have 4 joints and a total of 1000 N must pass through. You told us that mesh size has little or no affect on the force/moment passing through, so what parameters affects it? Geometry? Shape? Will changing the behavior (rigid/deformable/beam) change it? (I have also seen a change in force distribution to, for example, among the 4 joints where total force of 1000 N needs to pass, when the joint behavior is changed. Is this always true?.

[Rameez_ul_Haq]

Sir, your last paragraph suggests that you understood my point of view. As I also mentioned in my previous comment, that linking any two remote points (each scoped to a specific geometry) using constraint equations will have a force and moment transfer between them. Is it always the case? Consider the currently discussed example for instance. When I put a single constraint equation linking RP1 and RP2, making them displace by equal distances along X direction, will there be a force and moment transfer between them because of constraint equation? If yes, then how can I avoid this, since I only want the force and moment transfer to occur from the parts of solid beams connecting each other? Or the constraint equations need to exactly imitate that any joint constraint equations in order for the force and moment transfer to occur?SEPARATE CONCERNnSo what is the force passing through a joint dependent upon? For example if there are 4 joints and a total of 1000 N need to pass through them, so what are the parameters which decides the portion of total force passing through each of them? You already said that Mesh is not a influencing parameter, as it minutely affects the force reaction results. Is ratio of faces' areas in one joint to other joints a parameter? What if we make change the joint behavior (from rigid to deformable or beam), what else?nThank you.

[Rameez_ul_Haq]

How does switching from 'Joint Element' to 'Contact/Direct' in the option of Solver Element Type under the fixed joint definition, affect my solution?n

[peteroznewman]

FRAME STRUCTURE nDo some research into Exact Constraint Design. There is a book by Douglas Blanding, whose book I have read. This is a body of knowledge that helps you design structures that have exactly six ground constraints (among other concepts). The Pinned-Roller constraint pattern described above is one example of an Exact Constraint design. In that example, there is a revolute joint at Rp1 so there are zero moments about Z. There is a 1 DOF Y support at Rp2 so there are zero forces along X and Z and zero moments about any axis. Since the applied load has a zero component in the X and Z directions, by static equilibrium of the free body diagram, we know there is going to be zero reaction force in the X and Z directions at Rp1. So you know before you solved anything the forces along X and Z are zero and the moments about Z are zero. All the stiffness in the X direction and rotations about the Z axis are coming strictly from the structure and none of the stiffness is coming from the ground. That is true whether you use a Constraint Equation to transfer the fixed point to the midpoint between Rp1 and Rp2 or whether you leave the fixed point at Rp1.nSEPARATE CONCERNnWhat determines the force going through each joint? Let's take your three link example above using the Pinned-Roller constraint pattern. Say there is a fixed joint at each end of the horizontal link. If you have taken a Statics course in Engineering school, you will know what a free body diagram is, and how to write the Static Equilibrium equations: Sum of the Forces = 0 and Sum of the Moments = 0. nSum of the Forces in the Y direction gives you equation (1) RFrp1 + RFrp2 = FORCE.nSum of the Moments about Z at Rp1 gives you equation (2) FORCE*Df = RFrp2*Drp2nYou can use equation (1) and (2) to solve for the two unknown reaction forces, RFrp1 and RFrp2.nOnce you have solved for those two unknowns, you can split the structure at the fixed joints at each end of the horizontal link. Now you have three new free body diagrams, one for each link. Additional Static Equilibrium equations can be written for each free body diagram to solve for the unknowns at each joint. You can do all this as hand calculations. You don't need ANSYS to do any of this calculation because this is what is called a Statically Determinate problem. But you can build this model in ANSYS using Beam elements and Fixed Joints and extract out the reaction forces and joint forces to check your hand calculations. Note that if you have the Fixed-Fixed support constraint pattern, that is called a Statically Indeterminate problem and it is much easier to build a model in ANSYS to get the results than it is to do a hand calculation. The reason is that for Fixed-Fixed constraints at the base, the magnitude of the X direction forces at Rp1 and Rp2 is another unknown, but the value of that force depends on the stiffness of the structure. Note that we did not need to know the stiffness of the structure for the Pinned-Roller constraints.nLAST QUESTIONnThis thread already has two topics intermingled. Please start a new discussion to ask your last question, Fixed Joint vs Bonded Contact.n

[Rameez_ul_Haq]

Hello sir, can you kindly guide me on how to decide the radius of beam when selecting the beam behavior for a fixed joint? What does the radius of beam behavior mean and how does it affect my solution? For the beam connection itself, I use the radius of the beam equal to that of the holes which are being joined together using beam. However, if I select the beam behavior for a beam connection, there it is needed to input the radius of beam behavior again. Should these two radiuses have to be different? How to select the beam behavior radius? Why would it be needed to have different materials for the beam connection and the beam behavior?n

[Rameez_ul_Haq]

Hello there. If you can guide me on this puzzling thought, I will highly appreciate that.nFor example, I have this geometry.nThere exists a Fixed DEFORMABLE joint in between them. I apply some loadings to this geometry and I observe the results. I will see that the reference and the mobile hole surfaces will be able to locally deform (with no extra artificial stiffness) since the fixed joint type is Deformable. But at the same time, since the joint is fixed, the two holes' surfaces are forbidden to do undergo a relative motion. However, the elements, and therefore each of the hole surfaces itself, do deform and this deformation can be of different sizes on each surface. Does this indirectly implies that the reference and mobile surfaces are actually making a relative motion, although they are connected through a fixed joint. nSecondly, can you kindly educate me on how to make the reference and mobile surfaces of this fixed joint to be partially deformable? I mean like they might be able to deform in certain degrees of freedom but not in all. For example, each of the hole surfaces (between which fixed joint is constructed) cannot shrink but can expand.nThank you.nn

[Rameez_ul_Haq]

,an opinion from you on this one will be appreciated alot.n

[Rameez_ul_Haq]

Array, waiting for your reply here n

[peteroznewman]

nTo answer the second question first, you can't have a joint where the hole surfaces can deform only by expanding and cannot shrink. If you want to simulate the effect of a pin in the hole, then model a pin in a hole.nIn a Fixed Joint with the behavior set to Deformable, each surface can deform, but the weighted average displacement of one surface is mathematically equal to the weighted average displacement of the other surface. So the two surfaces are fixed, on average. If you want every node on either surface to be absolutely fixed relative to every other node on either surface, then you would set the behavior to Rigid.n

[Rameez_ul_Haq]

Another thought, Mr. @peteroznewman, . Would like to have your view on this nDoes increasing the number of constraint equations within our model, for example by incorporating more and more fixed joints at different locations of the same two bodies, will increase by solution time or decrease it? I mean basically what we are doing is simplifying the solver equations, so that less number of unknown displacements needs to be found, so i think it will decrease it. Do you agree?n

[peteroznewman]

Adding Fixed Support or Displacement Boundary Conditions reduces the size of the stiffness matrix and so reduces slightly the solution time because those nodes (or some DOF on those nodes) are no longer unknown.nAdding Joints adds equations to the stiffness matrix and so increases slightly the solution time because the nodal displacement of the nodes in the joint is still unknown, but there is an additional constraint on what they can be.n