Ansys 19.1 – Timber frame shear wall using spring connections
-
-
Hello,
I am trying to model a timber frame shear wall panel. I get a few warnings and an error shown below:
I am using springs to simulate the members and sheathing being connected together. I have a feeling my issue is to do with the constraint set up. I want the bottom framing member to be fixed to the 'floor' and the rest of the members to simulate being connected together by nails. I don't want the panel to move out of plane. I do want the 'nailed' connections to have some degree of movement as it would in real life hence why I have used spring contacts.
Can anyone help me understand why the model will not solve?
-
Hello Connor,
I can help you, and I can be more effective if you put
UniHeriot WattResearch DissertationANSYS ModelsInventor ModelsAssembly1.stp into a zip file and attach that to your reply. Without this file, I can't show you how the geometry can be modified to make the model building a lot better.
Beams would better represent the nails than springs and there is a much cleaner way to do them, and that is by imprinting the Stud cross-section onto the Top and Bottom Rails. That way, instead of one end of the spring being scoped to the entire length of the Bottom Rail, it will just be scoped to the little piece of the Bottom Rail that is touching the Stud above it.
However, I notice that you also have Bonded Contact between the Studs and the Top and Bottom Rails. That is doubling up on what the beams are doing, so it would be better to delete the contact between the Studs and the Top and Bottom Rails. The beams will prevent them from penetrating each other, and they are free to tip and tilt on each other by bending the beam.
The Remote Force loads are all scoped to the same vertex, though they have different Z coordinates. This is the wrong way to go about loading the structure. Please describe what you want to accomplish and I will recommend how you can achieve that loading.
Regards,
Peter
-
-
Hi Connor,
When you say "point load" I understand what you mean, but that does not literally translate into load on a vertex. It is best to apply loads in a solid element model (as opposed to shell models on surfaces) on a face, and second best to an edge. Try to avoid applying loads to a vertex. However, relative to the overall size of the wall, picking an edge or face of the stud is very localized to the stud.
Imprinting
Right click on Geometry cell in Workbench and Edit in DesignModeler. Click Generate (F5). Expand the 19 Parts, 19 Bodies line in the Tree Outline. Pick all the parts in the DesignModeler outline, and RMB to Form New Part. Now you have 1 Part, 19 Bodies.
At this stage, the parts are going to be "glued together" during meshing. This is sometimes what you want, but in this case, you want to change the Shared Topology Method default from Automatic to Imprints. That will create a face on the long bottom and top rails at each stud. Close DM and Refresh Project in Workbench to bring the new geometry into the Model. Open the Model.
Now in Mechanical, you can create a Beam between the face on the rail and the face on the stud.
When you click the face, it puts one end of the beam on that face, but subtract off 0.3" (or add on the top rail) to offset the beam end, since the other end of the beam is going to be defined on a coincident face on the stud and you can't have a zero length beam. Add 0.3" to the bottom of the stud (or subtract on the top of the stud). Now you have a 0.6" long beam and that beam can bend with the stiffness of a steel cylinder that you define, maybe 0.05"
Since the beam is very stiff along its axis, there is no need for contact on the top or bottom of the studs to the rails.
What version of ANSYS are you using? Attached is an ANSYS 19.1 archive.
Regards,
Peter
-
Hi Peter,
I have modeled the beams in place of the springs but it appears it does not allow the stud and the bottom rail to spererate as it would in reality. Is this because the beam is too stiff or should it be a spring? As I would also like to fix the Sheathing to the studs either using a beam or spring. The connection between the stud and bottom and top rail is really only taking axial loads and the connection between the sheathing and stud is lateral loads, should these connections differ due to their loading? Also, the beam does not allow for a stiffness to be input but the spring does?
As for the vertical loads. I understand what you mean, but the vertical loads should be acting downwards through the centroid of each stud but should be applied to the top rail, above each stud. if that makes sense?
Above is the standard im trying to replicate. Ie the vertical loads.
Also is there any way I can speed up the analysis?
Regards
Connor
-
Hi Connor,
Using short beams allows the studs to rotate about each end. For example, with just the bottom rail and one stud connected with a beam, I can apply 0.25 lbf to the top of the stud and see a 10” displacement at the top.
The beam is acting as a spring. The 0.25 lbf for the 10" deflection was for a beam with a 0.05" radius. If you change the radius to 0.1" then the force to deflect 10" becomes 2.0 lbs and the stud starts to show some flexing. So the beam diameter and length control its spring rate. There are beam bending formulas if you want to know the exact spring rate.
If you zoom in on the bottom of the stud, you will see it is rotating.
This is not exactly what you want, you could offset the beam to align with the edge of the stud.
Here the beam was at the center of the face:
Now it is offset to the edge of the stud.
Here is the deformation of 10" at the top.
If you used Frictional Contact, you could get the same effect, but that would slow down the simulation.
The best way to speed up the simulation would be to change the sheathing from a solid model to a Mid-Surface. Then the sheathing is meshed with shell elements that are assigned the thickness of the sheathing. I have done that for one OBS panel.
Another way to speed up the simulation is if you have multiple cores on your computer.
The way to apply force to the top rail is to use DesignModeler. Create a plane on the top, create a sketch on that plane, and use a Face Split. I have done that at a 100 mm dimension from the end as shown in the Standard. This creates a line to apply the load to in Mechanical. You can see the Surface of the sheathing in the image below.
You can use beams to connect the sheathing to the frame. You need to create a point on the midsurface that represents the sheathing. While you can connect a beam to a point on a shell element on a surface, special consideration is needed to connect a beam to a solid element node on a vertex of the solid.
Beam and shell elements have nodes with six degrees of freedom: 3 translations and 3 rotations. Solid element nodes have only 3 translation degrees of freedom. If you cantilever a beam element off a shell, it will support load. If you cantilever a beam element off one node on a solid, it will fall over, since there is no rotational stiffness on a single node on the solid element. However since one end of the beam is on the shell, this may work for your model. (When you have to cantilever beams off of solids, you have to pick a face and make a bonded contact between the face and the beam vertex.)
Use DesignModeler to create a point on each side by creating planes to slice the sheet and rail and stud along their centerplanes where I imagine a nail would go. In the image below, I have hidden the face of the surface body in the corner of the sheathing to show the beam going between the two vertices.
The top rail is now 4 bodies, so they need to be put in their own part. The stud is now 2 bodies, so put them along with the web and the other stud into a part called Stud1. With Shared Topology set to Automatic for Stud1, those bodies will be held together by sharing common nodes at the coincident faces, so there is no need for bonded contact to hold them together. That will speed up your simulation slightly.
However, now the Imprints described in the previous post can't be used to cut out a small piece of the bottom rail. Instead, create a plane and make a sketch to use Face Split to form a rectangle at the bottom of the stud for the beam to be connected.
Finally, I added two Remote Displacements. The each have zero displacement for the X coordinate. Those act as the lateral supports allowed for in the Standard, and one of them is the Racking Load, which is input as a displacement. You use the Force Reaction to measure how much force is used to rack that end by the entered displacement.
That is a lot to absorb. Good luck!
Regards,
Peter
-
-
-
-
-
-
Hi Connor,
Under Mesh Details, I set the element order to Linear to get rid of the Mixed Mode warning. I don't know if that was required or not.
I also saw that the nails only fasten the first sheet to the rails, so I suppressed the second sheet.
I fixed up the BCs and it ran. Were you going to run some nails down the studs?
Regards,
Peter
-
-
-
-
-
You may have seen by now that the problem was along the top rail. It will be best if there are two elements through the thickness of the top rail.
Click on Mesh Details, and under the Sizing Branch, set Adaptive to No, then lower down, set Proximity to Yes, then for Number of Elements across gap set that to 2. And set the Proximity Min Size to 10 mm.
Then you get a good mesh on the top rail. Then you must add an Edge Sizing on all the edges of the Studs. Use the Box Select method. You have to set the Behavior to Hard to get it to take.
-
-
-
-
Hi Connor,
You didn't request 2 elements across the gap, only 1. You can also change back to Quadratic Element Order, that helps it to finish.
You are slowing down your solution somewhat by requiring 12 steps to get to the final load of 54 kN. Each step by default is taking 4 substeps to get there. If instead you only requested 4 steps of 13.5 kN each increment, it might get to the final load with less total increments.
Looks like one of the studs is buckling.
Regards,
Peter
-
-
-
-
-
-
-
Hi Connor,
When I run your model on a Full License, here is the summary.
--- Number of total nodes = 28239
--- Number of contact elements = 81988
--- Number of spring elements = 0
--- Number of bearing elements = 0
--- Number of solid elements = 25403
--- Number of condensed parts = 0
--- Number of total elements = 107391
The contact elements are causing your model to exceed the 32,000 element limit. They aren't created in Mechanical so you can't see them till the solver runs, then they are created, pushing your model over the limit.
If you delete all these bonded contacts, the solver will start.
However, the solver will fail because you need to add some beams to connect the studs to the OBS and to the rails.
You still have a row of nails on the top and bottom that you don't need. The bottom nails because the bottom rail is gone. The top nails because the top rail is sharing topology with the OBS as shown by the purple line at the intersection.
I reduced the mesh density and put back one bonded contact of top rail to studs and this will run. Archive 19.1 attached.
Kind regards,
Peter
-
-
Hi Connor,
You made the surface wider than the top rail. There is supposed to be a gap between the top rail and the midsurface of the OSB, but you made them touch.
Make the midsurface for the top rail equal to the width of the top rail and you will get the gap back and can use the nails to connect the two midsurfaces.
You can reduce the mesh density on the OSB and the Top Rail. If you have to, you can convert the studs into surfaces as described in a previous post. In that way you can certainly have a model that runs in the Student license limits.
Here are two studs, one has been converted into a midsurface model, with two different thickness assignments.
I used Combine on the three solids to make them one before I used Midsurface.
Regards,
Peter
-
-
-
-
Hi Connor,
The problem is the Beam is not connected to the Stud.
You can add a fixed joint between the end of the beam and the face of the stud.
Do this for the 10 beams at the top of the studs and the 10 beams at the bottom of the studs. There is some automation called the Object Generator that could do this, but you have to do some setup to make it run.
Kind regards,
Peter
-
Here you go, I made the 20 joints with some automation, but you need contact now.
I added Bonded contact to prevent the OSB from penetrating the Studs. You could add beams instead to simulate nails.
It solves to the end, but you have to do research on how to get the orthotropic material X direction to go along the top rail now that it is a shell mesh instead of a solid mesh. Here is a relevant post.
ANSYS 19.1 archive attached.
-
-
-
-
-
- The topic ‘Ansys 19.1 – Timber frame shear wall using spring connections’ is closed to new replies.
You are navigating away from the AIS Discovery experience