Ansys 19.1 - Timber frame shear wall using spring connections

  • 562 Views
  • Last Post 11 October 2018
  • Topic Is Solved
ConnorMcGlade posted this 21 August 2018

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?

Attached Files

Order By: Standard | Newest | Votes
peteroznewman posted this 11 October 2018

Hi Connor,

No problem. Please start a new discussion for the next set of questions.

Regards,

Peter

ConnorMcGlade posted this 10 October 2018

 Hi Peter, 

Your help has been incredible thus far, sorry for the long reply, I started a new job the day after my last post. Coming back to this now for the final push. 

 

Connor

peteroznewman posted this 09 September 2018

Hi Connor,

I made a video to show how to use the Object Generator to quickly make 20 Fixed Joints to connect the beam vertex to the stud face.

I put it in the Tutorial section so that it might be found by people looking for Object Generator.

Regards,

Peter

peteroznewman posted this 04 September 2018

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.

Attached Files

  • Liked by
  • ConnorMcGlade
peteroznewman posted this 04 September 2018

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

ConnorMcGlade posted this 04 September 2018

Hi Peter, 

I've added in some extra nails again for the studs and the other OSB. I now appear to get a pivot warning, why is this? Is it something I haven't restained?

See attatched 

Kind Regards

 

Connor 

Attached Files

peteroznewman posted this 04 September 2018

Make that surface the Active Component.

Click on the Pull Tool

Pick the Edge you want to move

Type U to use the Up To feature

Click on the side of a Stud.

The Top Rail will be level with the edge of a Stud.

ConnorMcGlade posted this 03 September 2018

How can I change the size of the surface?

peteroznewman posted this 03 September 2018

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

ConnorMcGlade posted this 03 September 2018

Hi Pete

Thanks for that, I got that to run!

Although now the top rail and OSB are now bonded, this does not replicate a nailed connection, is there a way of now replicating this? 

I have tried now putting beams to connect the studs to the ground rather than a fully fixed connection, but this is now causing me to exceed the problem limit. How can i get round this? I feel like were so close this now!! My aim is to get a model with sheathing fixed to the studs replicating a nailing pattern around the perimeter of both sheets an the studs being connected to the ground using beams so there is a stiffness on the uplift forces. Is this going to be possible with my size of model?

Kind Regards

 

Connor 

peteroznewman posted this 02 September 2018

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

 

Attached Files

ConnorMcGlade posted this 02 September 2018

Hi Peter, 

I think deleting the bottom rail then adding beams can be my next move! 

I'm trying to get the mesh right for this model now but still is not working, its now giving me the error that my node count is higher than 32k. Both my elements and nodes are less than 32k combined. I've seen your other thread about updating the geometry from source but still not working, I've shut the program down and opened it back up as well as clearing data and still is not working. What is wrong with the model?

Kind Regards

 

Connor 

Attached Files

peteroznewman posted this 02 September 2018

Hi Connor,

Connecting sheet bodies to solid bodies requires some care due to the fact that nodes on solid elements don't support rotations. It would be better to generate three sheets, assign a large thickness to the flanges and assign a small thickness to the web. If those three sheets are in a multibody part, then Shared Topology will connect them with shared nodes at the common edge. In bending and twisting, these three sheets will respond very similarly to the solid body version.

Regards,

Peter

  • Liked by
  • ConnorMcGlade
ConnorMcGlade posted this 02 September 2018

Hi Peter, 

That sounds like a good idea, whats your thoughts on going a step further and changing the webs in the studs to sheet bodies?

I'll let you know how I get on!

 

Kind Regards

 

Connor 

peteroznewman posted this 31 August 2018

Hi Connor,

In fact, beams are the most efficient way to model a structure. Using mid-surface models is the second most efficient and using solids is the least efficient way to model a structure, in terms of minimizing node count.

You should replace the top and bottom rails with sheet bodies at the mid-surface. Just keep the Studs, which are meshing very efficiently.  However, the bottom rail is Fixed to ground, so just eliminate the bottom rail and connect the bottom of each Stud to ground either with a Fixed Support, or a Beam!

Regards,

Peter

  • Liked by
  • ConnorMcGlade
ConnorMcGlade posted this 31 August 2018

Hi Peter, 

I've tried to no avail to get the nodes under my student limit. Is there any other way of modelling this to further reduce the problem size? I'm aware I'm already exceeding the limit without both sheathing parts. Could using the beams be using up too many nodes/elements? 

Regards

Connor 

ConnorMcGlade posted this 31 August 2018

Hi Peter 

Thanks for that, I'm struggling at the moment to try and get the nodes/elements under 32k, I think i may need to do some fiddling about to get a mesh that works under 32k

Connor 

peteroznewman posted this 31 August 2018

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

Attached Files

peteroznewman posted this 31 August 2018

Hi Jimmy,

I only know Structural simulations. I'm very much a beginner at this CFD stuff, especially with concentrations and mass transfer.

Fortunately, there are lot's of ANSYS experts on the site now!

Good luck, and please delete your post from this discussion.

I hope I can help next time.

Kind regards,

Peter

Jimmyhan posted this 31 August 2018

Hi Peter, I need your help, why not give me some suggestion for my simulation.https://studentcommunity.ansys.com/thread/set-source-and-source-coefficient-in-mass-transfer-simulation/?postbadges=true

ConnorMcGlade posted this 31 August 2018

Hi Peter, 

I tried that but I still get the same issue?

 

Regards

 

Connor 

Attached Files

peteroznewman posted this 31 August 2018

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.

 

peteroznewman posted this 30 August 2018

Hi Connor,

Click on Solution Information and in the details window, type 3 for Newton-Raphson Residuals.  Then click Solve. After solving, there will be 3 plots under the Solution Information folder. The maximum value on those plots shows you the location where the solver can't get convergence. It needs more elements at that location. Add mesh controls to make smaller elements at the location of the maximum N-R Residual plot. I will reply with that plot that when it finishes solving.

Regards,

Peter

  • Liked by
  • ConnorMcGlade
ConnorMcGlade posted this 30 August 2018

Hi Pete, 

I thought that, that makes sense to me. Would you mind looking at the attatched file above and seeing why it will not solve?

I'm currently running 4 cores. 

Regards

Connor

peteroznewman posted this 30 August 2018

Hi Connor,

You need the bonded contact between the Rails and the Studs, but you can replace that with beams like we did at the very beginning.

I did suppress the bonded contact between the Flange and the OSB since it was connected with nails at the top and the bottom rails. You can run it with that contact on for a different result.

How many cores does your computer have?

Regards,

Peter                                                                                                                                                                                                                                                                                                                                                                                                                                                                                                                                                                                                                                                                                                                                                                                                                                 

  • Liked by
  • ConnorMcGlade
ConnorMcGlade posted this 30 August 2018

Hi Peter, 

My model seems to be taking a while to solve, changing to linear has stopped that error, could the long solve time be due to contacts? I still have bonded contacts between the flanges and the top and bottom rails, is this correct? I also have had to suppress bonded contacts between flange and OSB but your model did not appear to have these?

Yes the intention is to have nails running the perimeter studs and rails as well as the internal studs. I then plan on creating several models with difference nail spacings i.e 50mm, 100mm and 150mm. 

I have tried to run the analysis but it seems to be something to do with my constraints although its seems to be restained fine to me, im not sure why it wont solve. 

I have attatched the file 

Regards

 

Connor 

Attached Files

peteroznewman posted this 30 August 2018

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

 

ConnorMcGlade posted this 30 August 2018

Hi Peter, 

 

Sorry for the slow reply, your videos have been extremely useful, I've followed them both through fairly easily, although when I come to the last stage my mesh appears to be solid and not a surface, why is this, is it something visual or something i havnt done? 

I really do appreciate the time you've taken here to create these solutions! 

 

I have attached my archive 

Attached Files

peteroznewman posted this 26 August 2018

In this video, Shared Topology is used to connect the beams to the sheet and solid.

Also, I see you have orthotropic material for the wood. This requires that you define two coordinate systems where each x-axis points along the length of the rail and spar respectively, so that the high stiffness axial direction of the grain is properly used.

 

You can show your appreciation by clicking Like below the posts that are helpful.

  • Liked by
  • ConnorMcGlade
peteroznewman posted this 26 August 2018

Hi Connor,

Here is a video on how to create a midsurface in SpaceClaim and a row of beam elements to represent the nails.

 

You can show your appreciation by clicking Like below the posts that are helpful.

  • Liked by
  • ConnorMcGlade
Show More Posts
Close