I am trying to model post-tensioned reinforcement in concrete. I am starting off (I assumed simply) by modeling the reinforcement as a truss element and then I intended on applying a temperature to the truss element to model the strain. Anyway, I can't seem to form a contact between the truss element and the solid.When I run the model it looks like the reinforcment is a straight line between the two end surfaces.
I found the following discussion that appeared to be relevant:
I am currently just playing with a linear model, nevertheless, I can't seem to get a setting that indicates the truss element should be contacted along the length.
I was originallly trying to run the truss element internally, that didn't work. Then I put on the external surface of the solid and I still didn't find any more luck.
Help is much appreciated...
Well, this stikes me a bit odd, but the option does show up if I make the DS a MES. I guess I will hack through that now.
Hi,
In a static analysis, you should connect the truss member that you've defined to the solid elements (ideally with the "Spider" technique.
Looks like the text is missaligned on the page.
To test, I simply created a block with a through hole (in solid elements)
On each side of the hole i've placed a spider (lines connecting the nodes on the edge of the hole to the centre of the hole, "contact" tool allows a faster creation). Each spider is in a separate part and defined as a "Rigid" element.
The two centre nodes at each side of the hole are connected to each other by a truss element defined as a new part, and given the desired free temperature.
In the analysis parameters, specify the default nodal temperature and activate the themal multiplier by entering "1".
It works as expected for me and shows the stress
Regards
Shakeel
Hi and welcome to the forum,
The problem is that you have one truss element; you need multiple truss elements. In simulation and finite element analysis, elements are connected together through the nodes. So if you have one truss element that connects to the solid at the extremities of the solid, then you have a rod connected at two point.
You will need to create the model and mesh so that you have a straight line (assuming the rods are straight) at the location of the rods. This is easy with a hand-built model because you control the mesh. With a CAD model, you will need additional parts so that the volume of concrete is split where you need the rods to be. Depending on the capabilities of your CAD application, you may be able to split the surface where the rods or needed; otherwise, you would need separate parts for each section of concrete. (See the attached image.)
Once the model is made, creating the rods is easy.
Hmmm.... This is all very helpful. I have not done concrete reinforcement in Autodesk Simulation, so forgive my ineptitude.
Let me broaden a little bit, attached is the figure. Not a trivial amount of reinforcement and it will lead to a lot of surfaces in the manner prescribed previously. I have been debating on how to handle it. My objectives are to evaluate the following:
1) Understand the natural response (first 5-10 modes)
2) Understand the forced response under an inputted time history
3) From the transient time history make evaluations where to install strain gages
4) Eventually take measured strain and acceleration data and make observations from analytical model (linear model)
5) If not to painful, make observations of 4) in a nonlinear model.
I had debated on a number of approaches, I thought by chance drawing lines and making contact with the solid would be the easiest. Not looking like it.
Next thought based on this input, but not reseaching it yet would be to slice the solid at each reinforcing elevation and install a shell layer to be the reinforcing- more of a smear reinforcing approach.
I am using Autocad Autodesk to build my initial 3D solid. I have access to Inventor Fusion 2012, but I don't have any seat time in that.
So would a smeared approach work best over a discrete reinforcement model? If smeared then, a shell layer to do so? I did not see a whole lot for concrete on the discussion boards, so flying a little blind.
Hi,
What is the total length of the Girder to be considered?
What type of behavior between the concerete and bars will be along the length ? I mean the pretension will be transfered only on the girder ends or through out the length (perfect adherence of the trusses with the concrete)?
Regards,
Shakeel
Here is what I find to be the best suited method :
1. Create the sketch of the section, with points where you've your Reinf. bars. You can do it either directly in ASim or ACAD and import it in ASim
2. create a 2D mesh to get a node at each of your Reinf locations (I had to move the nodes to get the nodes at the Reinf locations)
3. Extrude the 2D mesh along the length of the Girder to get your 3D mesh (Select lines > right click>Move/Copy and use join option)
4. From the 2D projection view select all reinf locations using Line Selection tool (This should select all lines representing the Reinf bars)
5. Duplicate all these lines and attribute a new part number.Attribute this part the properties of the trusses to represent Reinf.
You have your Reinf bars modeled in your solid with a perfect adherence with concrete 🙂
Regards
Shakeel
Responses:
1. What is the total length of the Girder to be considered?
130 ft
2.What type of behavior between the concerete and bars will be along the length ? I mean the pretension will be transfered only on the girder ends or through out the length (perfect adherence of the trusses with the concrete)?
True behavior of cast in prestressing steel would that it would effectively be transferred in at the ends, albeit it takes place over a few feet. So there is some slip in the interface between the steel and concrete in the end. Kind of complex and I don't aim to model this behavior. If adding steel had been trivial then at a basic level it just approves the appearance, (i.e. the level of detail is obvious). On a secondary level, an outlying goal would be to use the model to evaluate cracking taking into account the steel resistance in a nonlinear model.
3. With regards to your suggestinon of modeling technique. I like the idea of sketching in the reinforcing bars, although in practice it starts to become a question of tradeoffs. First, a straigth "create 2D mesh" does not result in a nice gridded symmetrical mesh, so having asymmetric non-uniform spacing of prestressing seems less than ideal. Now, I could break the shape up into rectangular sections and do a structured mesh. This is reasonable, but makes wonder if I really want to do this. I had tried layering in the slicing and creating a membrane layer for the reinforcing--smeared reinforcing layer, but after a long analysis period found that bonded contact didn't seem to tie as I had assumed it would.
I had saw another software program do this a little more elegantly, but Autodesk Simulation is the hammer I have. If having the reinforcing in the model is critical then it looks like I need to drill out the holes for it, draw it in discretely, and then attach it with a spider technique.
I nevertheless very much liked the advice. It was very instructive and appreciated. It looks like I can't effectively get the contribution of the prestress using a linear frequency response, so i think I need to use MES and I'll just add in external loads to model the prestressing, pluck the beam, and look at the response-- for now. I will cross the bridge of discreetly modeling steel later, if possible.
Hi,
I am confused on a couple of points in your reply. You wrote that the pretensioning is effective only over a few feet at the end, but you do not aim to model that behavior. If that is the case, then attaching 1 truss element at the ends of the 130 ft beam for each rod is easy to do. Actually, you can model the attachment over the last X feet relatively easily as follows: (this method just came to mind )
The other item is where you mentioned that you cannot get the natural frequency (I believe that is what you meant by "frequency response") and take the prestress into account. I think you can get what you want by using the analysis type "Natural Frequency (Modal) with Load Stiffening".
Thanks for your reply John.
I actually think I tried to execute this method originally, similar to the manner you describe. The problem I encountered was that the truss elements are ONLY connected at the end. The beam mesh doesn't seem to know that they are there internally. Thus and exaggerated deflection diagram shows the truss element absolutely straight, and the beam deflecting under gravity load (the load case that I reviewed it under). I didn't see any difference in steps that would suggest any large difference, but if you feel I indeed missed something, I will track back through it.
Regarding your second point, yes, I meant to state Natural Frequency.
Thanks,
Rich