Modeling Tips

Applying In-Plane Moment to Plates

Occasionally you may need to model an applied in-plane moment at a node connected to plate elements. The plate/shell element cannot directly model in-plane rotations. One way around this is to model the in-plane moment as a force couple of in-plane forces. You would replace the applied in-plane node moment at 1 node with 2 or 4 in-plane forces at 2 or 4 nodes , which would produce the same magnitude in-plane moment. See below:

This might require re-meshing the area receiving the moment into smaller plates so that the load area can be more accurately modeled. If a beam member is attached to the node and will be used to transfer the moment, than you will want to look at the topic Modeling a Beam Fixed to a Shear Wall below.

Modeling a Beam Fixed to a Shear Wall

Occasionally you may need to model the situation where you have a beam element that is fixed into a shear wall. A situation where this may occur would be a concrete beam that was cast integrally with the shear wall or a steel beam that was cast into the shear wall. The beam cannot just be attached to the node at the wall because the plate/shell element does not model in-plane rotational stiffness. A fairly simple work around is to use rigid links to transfer the bending moment from the node at the wall as shear force to the surrounding nodes in the wall. See Rigid Links in the Modeling Tips section to learn how to create rigid links. This modeling method provides a more accurate analysis than trying to use a plate/shell element with a “drilling degree of freedom” which attempts to directly model the in-plane rotation. See the figure below:

The only trick to this method is getting the proper member end releases for the rigid links. We want to transfer shear forces from the wall node to the interior wall nodes without having the rigid links affect the stiffness of the shear wall. Notice from the figure that the I-node for all the links is the node connected to the beam element, while the J-nodes are the ends that extend into the shear wall. The J-ends of all the rigid links should have their x, Mx, My, and Mz degrees of freedom released. Only the y and z degrees of freedom (local axes shears) should be connected from the J-ends to the interior wall nodes . This release configuration will allow the shears to be transferred into the wall, but the wall stiffness will not be adversely affected by the presence of the rigid links.

Modeling a Cable

While there is not a true “cable element”, there is a tension only element. A true cable element will include the effects of axial pre-stress as well as large deflection theory, such that the flexural stiffness of the cable will be a function of the axial force in the cable. In other words, for a true cable element the axial force will be applied to the deflected shape of the cable instead of being applied to the initial (undeflected) shape. If you try to model a cable element by just using members with very weak Iyy and Izz properties and then applying a transverse load, you will not get cable action. What will happen is that the beam elements will deflect enormously with NO increase in axial force. This is because the change in geometry due to the transverse loading will occur after all the loads are applied, so none of the load will be converted into an axial force.

Guyed Structure (“Straight” Cables)

You can easily model cables that are straight and effectively experience only axial loading. If the cable is not straight or experiences force other than axial force then see the next section.

When modeling guyed structures you can model the cables with a weightless material so that the transverse cable member deflections are not reported. If you do this you should place all of the cable self-weight elsewhere on the structure as a point load. If you do not do this then the cable deflections (other than the axial deflection) will be reported as very large since it is cable action that keeps a guyed cable straight. If you are interested in the deflection of the cable the calculation is a function of the length and the force and you would have to calculate this by hand.

The section set for the cable; should be modeled as a tension only member so that the cable is not allowed to take compression. See T/C Members for more on this.

To prestress the cable you can apply a thermal load to create the pre-tension of the cable. See Prestressing with Thermal Loads to learn how to do this.

Modeling Composite Behavior

Occasionally you may want to model a structure with composite behavior. A practical situation where this arises is with composite concrete floor slabs, which have concrete slabs over steel or concrete beams. Another common case where composite behavior may be considered is where you have a steel tank with stiffeners. The stiffeners might be single angles or WT shapes.

The most accurate way to model this behavior for composite floor systems is to use a program (such a RISAFloor) that was created explicitly for this purpose. If that is not an option you may want to use an arbitrary member with an effective moment of inertia, I_eff, calculated according to the AISC or Canadian code provisions. This method has the advantage of being able to account for the effects of partial composite behavior, while the methods described below assume perfect connectivity between the steel beam and the concrete slab.

If you have already modeled the concrete deck with plate elements, then the situation can be quickly modeled for horizontal beams by using one beam modeled as a physical member and also using Analysis Offsets. The beam would simply be drawn along the plates/nodes for the composite section. This method has the advantage of being very fast to model but it also neglects the depth of the concrete in computing the total vertical offset between the centerline of the beam and the centerline of the slab. Note that you have to have an appropriate number of nodes along the span of the beam to model the shear transfer between the slab and the beam. A more refined (and complicated) method using rigid links is described next.

An example of a plate/beam model with composite action included using rigid links is shown here:

Note that beams and plates are each modeled at their respective centerlines. It is this offset of the beam and plate centerlines that causes the composite behavior. The distance between the centerlines is typically half the depth of the beam plus half the thickness of the plate elements. If the beam is an unsymmetrical shape, like a WT about the z-z axis or a single angle, then you would use the distance from the flange face to the neutral axis.

As shown above, a rigid link is used to connect each set of nodes between the beam and the plates. This rigid link is fixed to each node and therefore has no member end releases. See Rigid Links in the Modeling Tips section to learn how to create rigid links.

Graphical editing offers the fastest way to model composite action. It is usually best to model the plates with an appropriately fine mesh first. Then you would copy the plate nodes that are directly over the beam down to the centerline elevation of the beams. Next you would draw your beam to the two outer nodes at the beam centerline elevation.

There are a number of ways to build your rigid link member between all the corresponding plate and beam nodes . A good way to connect all the links is to generate grid members (Grid Member Generation). You can also draw the first one and then copy it along the length of the member.

Now perform a model merge. If you have used finite members rather than Physical Members the merge Model Merge will break up finite element beams at all the intermediate locations. See Model Merge for more information. If you’re using physical members, performing the model merge will clean up duplicate nodes and members but not break up the beam member since the links are automatically attached to Physical Members as long as their node lie on the member.

Modeling Inclined Supports

You can model inclined supports by using a short rigid link to span between a node which is restrained in the global directions and the item to receive the inclined support. See the figure below:

The rigid link should be “short”, say no more than 0.1 ft. The member end releases for the rigid link at node “B” are used to control which degrees of freedom are pinned or fixed in the inclined directions. This works because the member end releases are in the local member axes. See Rigid Links in the Modeling Tips section to learn how to create rigid links.

The section forces in the rigid link are the inclined reactions. Note that you need to make sure the rigid link is connected to the members/plates at the correct inclined angle. You can control the incline of the angle using the coordinates of nodes “A” and “B”. You can also rotate the rigid link to the proper angle.

Modeling One Member Over Another

Occasionally you may need to model the situation where one member crosses over another member. A common situation where this occurs is in the design of framing for crane rails, where the crane rail sits on top of, or is hanging beneath, the supporting beam. See the figure below:

The two beams are each modeled at their correct centerline elevations. Both the top and bottom members need to have a node at the point of intersection. The distance between the nodes would be half the depth of the top beam plus half the depth of the bottom beam. The method to model this is to connect node A to node B is with a rigid link. The member end releases at the A or B end can be used to control which degrees of freedom get transferred between the beams. For example, if Beam A is free to pivot over Beam B then you would apply a Pin end release to the top of the rigid link, and a Fixed end release to the bottom of the rigid link. Don't pin both ends of the rigid link though, because then there can be no shear transfer between the beams. See Rigid Links in the Modeling Tips section to learn how to create rigid links.

Reactions at Nodes with Enforced Displacements

The reaction at an enforced displacement can be obtained by inserting a very short (.02' or so) rigid link between the node with the enforced displacement and any attached members. The member forces in this rigid link will be the reactions at the node with the enforced displacement. It is helpful to align the link to be parallel with one of the global axes, that way the local member forces will be parallel to the global directions unless of course you are modeling inclined supports. See Rigid Links below to learn how to create rigid links.

Rigid Links

Rigid links are used to rigidly transfer the forces from one point to another and to also account for any secondary moments that may occur due to moving the force. This is in contrast to using the tether feature for nodes where the forces are shared by 2 or more node degrees of freedom (DOF), but any secondary moments are lost when tethering the nodes . Tethered nodes actually share common DOF and so do not account for the distances between them. Rigid links do not have any practical internal deformation, I.e. there is no differential movement between the I-node and the J-node . Rigid links may be used to model situations such as compositebehavior or beams fixed to walls modeled with plate elements. They are also useful for getting information such as reactions at inclined supports or reactions at nodes with enforced displacements.

Make a Rigid Link

To make a Rigid Link:

On the General tab of the Materials spreadsheet:
1. Create a material Label called “LINK”.
2. Enter “1e6 (ksi)” for the value of E.
3. Blank out the value for G by going to that column and pressing the space bar.
4. Double check that the Density is set to zero.
5. Leave all the other values as their defaults.
On the General tab of the Section Sets spreadsheet, create a section set Label called “RIGID” with the “LINK”Material.
Move the cursor to the Shape column and hit your space bar to erase the information in this field.
Set the A,and Iy, Izand Jvalues to “1e6 (based on units of inches)”.
To make a rigid link, on the Members spreadsheet create a member that references the RIGID section set created above.

You can control which DOF are transferred through the link by using the member end releases.
Note:
- The density is set to zero in case the self-weight is used in a loading condition. If the density is left as the default then any gravity loading would cause the rigid link to add a very large load into your model due to it’s large area.
- To keep the model merge from deleting your rigid links, be careful not to create links whose lengths are less than your merge tolerance.
The weight density should be set to zero in case self-weight is used as a loading condition. If the material used is not weightless, then any gravity loading would cause the rigid link to add a very large load into your model. (Gravity load is applied as a distributed load with a magnitude equal to the member area times the weight density).

For models with very stiff elements, like concrete shear walls, the rigid link may not be rigid in comparison. If you see that the rigid link is deforming, then you may have to increase the stiffness of the link. The easiest way to do this is to increase the A, Iy, Iz, and J values for the RIGID section set. Make sure that the combination of E*I or E*A does not exceed 1e17 because 1e20 and 8.33e18 are the internal stiffnesses of the translational and rotational Reaction boundary conditions. If you make a member too stiff, you may get ghost reactions, which tend to pull load out of the model. (The total reactions will no longer add up to the applied loads.)

Solving Large Models

Large models are those where the stiffness matrix size greatly exceeds the amount of available free RAM on your computer. Solving large models can take a long time, so it is useful to have an understanding of what steps can help speed up the solution. The time it takes to solve a model is dependent on several things; these include the bandwidth of the stiffness matrix, the number of terms that need to be stored for the stiffness matrix, and the amount of RAM in your computer.

A bandwidth minimizer is used at the beginning of the solution to try to reorder your degrees of freedom to get a reduced bandwidth stiffness matrix size. Sometimes, however, the bandwidth minimizer can be fooled and will give a poor matrix column height and a huge number of matrix terms.

If you are getting a stiffness matrix that is larger than you would expect and you don't think that you have any modeling errors, you can try a few things to reduce the bandwidth. The first thing you can try is to sort your nodes . Typically you will want to sort your nodes on the Coordinates spreadsheet from “Low to High” in the 2 lateral directions and then lastly in the vertical direction. After you sort your nodes , try to solve again and check the matrix size. The order of sorting depends on the model, so you might want to try a couple of different combinations and check the model each time. Sometimes, sorting the nodes will result in cutting the height and number of terms by a factor of 2.

You will also want to make sure you don't have separate structures in the same model where one is big and the other small. You will get a very large matrix height if the bandwidth minimization starts on the small model and then jumps to the big model. Instead, you will probably want to split these into 2 separate files.

The amount of “address space” available to solve your model is based on several things: the amount of RAM in your computer, the amount of free hard disk space, the operating system, the Virtual memory settings in the Windows Control Panel, and the internal limitations of your operating system.

If you get an error that states “You have run out of memory, try increasing your virtual memory…” you will want to note the amount of memory that was requested at the time versus the amount that was available. This amount should displayed along with the error message. This amount will give a starting point from which you can increase the available address space. You may need to increase the amount of Virtual Memory so that you have enough address space to run the model and your other applications. (You typically do this by double clicking on “My Computer”, then “Control Panel”, then “System”. Within the System options, you would click on the “Performance” tab and then you click on the “Virtual Memory” button.) Make sure that you are specifying more Virtual Memory than is needed to solve your model.

There is an internal limitation to the amount memory that Windows will allocate to the RISAProgram. Within a 32 bit addressing space, Windows has a basic limit of 4 Gigabytes. Of that, they reserve 2 Gigs for the operating system. Therefore, RISA can only use a maximum of 2 Gigabytes with large models (where the stiffness matrix alone is well in excess of 1.0 Gigs), your only option may be to re-model your structure using fewer degrees of freedom.

Ways to Minimize the Memory Use

Keep in mind that many of these solutions may result in a decreased accuracy of your solution

Set the Number of Sections and INTERNAL Sections to a minimal amount. This can be done via the Model Settings - Solution tab.
Set the Mesh Size for wall panels (if they exist in your model) to a larger value. This can be done via the Model Settings - Solution tab.
Solve fewer load combinations. It is almost always possible to reduce the total number of combinations by inspection. Engineering judgment can help determine which load combinations will not control for your structure.
Check to see that you are not causing an overly tight mesh for wall panels (if they exist in your model) by your modeling practices. This can cause a large amount of internal plates to be created and tax the solution. See the Wall Panels - Tips For Ensuring a Healthy Mesh section for more information.

Modeling a "Gap" (Expansion Joint) Between Structures

A gap element is a member that mimics the behavior of a gap or expansion joint between adjacent structures.

While RISA does not offer the capability to directly create a gap element, one may be indirectly created using the properties of the member and an applied thermal load. The concept is to place a ‘shrunk’ member between adjacent structures. The shrinkage of the member is achieved with a negative thermal load, in the form of a member distributed load.

The amount of shrinkage should be equal to the width of the gap, such that the structures act independently until they move close enough to each other to ‘touch’ and thereby transmit loads to each other. To calculate the thermal load required for a gap use the following formula:

Where:

ΔT = Applied thermal load

Gap = Distance between two structures

L = Length of gap element

α = Coefficient of thermal expansion

In order to prevent the gap element from ‘pulling’ its connected structures towards it due to shrinkage it must be defined as a ‘compression only’ member under the advanced options tab. It is also advisable to define the gap element as a rigid material such that the amount of load it transfers once the gap is closed is not affected by elastic shortening.

Lastly, in cases where the applied temperature would need to be of an extraordinary magnitude, it might be useful to increase the coefficient of thermal expansion of the material such that a smaller temperature load would achieve the same shrinkage.