Regarding 3D geometry preparation, it is unnecessary to be REVIT, any 3D software will do. AutoCAD, Rhino, Dynamo, Grasshopper, Design Modeler, or SpaceClaim,....etc. all will do. You choose whatever you have access to and are comfortable with. In case you choose SpaceClaim as your primary tool for 3D geometry preparation, first you should understand the workflow by at least following what has been shown in this video to the point where you get the picture of what data format (e.g. solid or curve) that required for nonlinear analysis. After that, regarding the how-to in SpaceClaim to obtain the required data format (solid/curve), there are already excellent SpaceClaim trainers who show various approaches to creating 3D models, Google/KZfaq search will help in this regard.

I just have tested with WB2022R2 and all the rebar models (DWG) can be imported into Spaceclaim just fine.

The 2021 version does affect the analysis results. The workflow needs to be modified according to details described in the pinned comment when using the ANSYS workbench version later than 2019. I would recommend creating the new material data for the new component such as steel plates. Even though the mechanical property of steel plates might be similar to rebar, it is good practice to separate material assignments. The material definition (both linear and nonlinear) and assignment of the steel plate could be done directly on the workbench user interface and not require any additional APDL command. Use CEINTF only for something that is embedded inside concrete such as rebar. For the steel plate that is only attached to the concrete's face and not embedded inside the concrete, just use bonded contact. If the concrete beam is subjected to non-reversal loading then you could simply attach the steel plate (solid or shell) element to the concrete surface. SOLID65 is not an option if the concrete beam is subjected to reversal loading because the material model can not be damaged/degraded. And if the delamination is neglected, then the bonded contact could also be applied. In practice, it is easier to consider delamination separately, not in FEM. The delamination interface between concrete and steel plate could also be done in ANSYS but that is not my expertise to provide an opinion. Or if the steel plate has been installed after the reinforced concrete beam is already damaged as a means of strengthening, using SOLID65 might not provide accurate results due to lacking strength degradation on its own. The modeling of concrete in ANSYS could be done in many ways, each has its own strength and weakness. The workflow in this video is tuned and suitable for practical use of real-life structure but may not be good for research purposes. There are mainly three groups of how to model concrete in ANSYS: 1. Drucker Prager concrete, Menetrey Willam 2. Micro-Plane model including CPT215 3. SOLID65 The Microplane model and CPT215 are superior to any other concrete model in terms of the compressive degradation and tension softening which by far superior to the SOLID65 concrete model. It is also compatible with the ANSYS's reinforcement feature that would allow the user to handle complicated rebars with ease. Not to mention the potential to capture reverse loading (cyclic) behavior if parameters are properly tunned. Menetrey Willam and Drucker Prager concrete can also get along with the new ANSYS reinforcement feature. Unfortunately, Menetrey Willam is not as good for general purpose as what ANSYS's developer trying to promote, also Drucker Prager concrete model. In order to properly utilize the superiority of the Microplane model and CPT215, there is a price to pay, its parameters. For example, there are 12 parameters involved with the Coupled Damage-Plasticity Microplane Model. After parameters tunning, the model could be used for a specific behavior those parameters tuned for. Applying the parameters that tuned for a specific behavior to another could easily lead to wrong predictions. For laboratory purposes, the Microplane model and CPT215 can be really useful. But not much for practical use. At the moment, there is no way to generalize the Microplane parameters to serve a general purpose for structural concrete. Or even such a thing exists, it is not yet generally well established or well published. Hence, Microplane models and CPT215 are not good options (yet) for general concrete structures. It needs some more time for the model to be fully explored. Once those parameters technology is well established, I will also switch to the Microplane model, but not for now. Since the content in my channel is intended for practical purposes and aimed to be used to solve real-life structures such as building and bridge structures. For now, SOLID65 is the most reliable concrete model for general purposes. And the SOLID65 weakness such as incapable of degradation or incapable of reverse loading is not the problem in practice because there is already a well-established method to handle that in real life. RemarK: It looks like SOLID65 is no longer maintained by ANSYS's developer and it already lost a few features that it had before. It seems SOLID65 is on the way to obsoleteness.

Regarding concrete beams with openings, a google search for the author Kiang-Hwee Tan should be a good start.

Sir can you help us with our project we can pay you​@@ThanaponBuamongkolChannel

"BEHAVIOUR OF REINFORCED HIGH-STRENGTH CONCRETE BEAMS WITH OPENINGS SUBJECTED TO STATIC AND REPEATED LOADINGS", Atif M. Abdel Hafez

You can also download from the link in the description.

Crack is no longer supported in the current version of ANSYS. The developer stops maintaining the legacy element (SOLID65).

@@ThanaponBuamongkolChannel Another problem I am recently facing that the force is way too much than the tutorial. Like it should be around 250 kN whereas I am getting 448 kN. What should be the solution? I am using WB2020 and the mesh size sub steps are similar.

@@asifmostafaanik5588 For WB2020 follow the pinned comments and fix the rebar mesh accordingly. Then try to suppress SOLID65 APDL command, if the results remain the same as when SOLID65 APDL command is active then that means the APDL doesn't register and something is wrong with the commands. If all above doesn't fix the issue, then maybe it's better to start all over again from new files and follow the steps in the video closely. Some details might be overlooked.

@@ThanaponBuamongkolChannel Sir, I followed your suggestion accordingly. Still the result was way out from the 250 kN point. Moreover, Suppressing the SOLID65 also ran the analysis however the force increased as expected, as the concrete is now structural steel. In WB2022R2 I am facing this type of problem. Previously when I used WB2019 did not had any issue. Can you help me by checking the model? I will be grateful, as I am showing this as a Validation for choosing SOLID65 as material model for a paper of mine. Thanks in advance. Link to the model is below. drive.google.com/file/d/1d4XwCEdwe9jWbhThBFvuEC81zAml_vfd/view?usp=sharing

@asifmostafaanik5588 I just take the file I have done when I use WB2019, the exact same file made in this video. Fix the rebar meshing as per pinned comments. And run the analysis on WB2022R2, the results are fine for BS-7 without doing anything else. For BS-8, I need to turn on the weak spring option (Analysis setting), and the results are fine as well. In conclusion, WB2022R2 is fine. Please note that the nonlinear analysis of concrete structures is one of the most complicated types that structural engineers will do in their routine life. There is no surprise that one would struggle to learn the workflow, and figure out what's wrong with the model. The learning process will take time. It took me years before I could proficiently use this workflow and publicly share the most efficient workflow as shown in this video. Try to figure out what you might have overlooked or missed from the workflow shown in the video, some very small details might cause a big change.

If you use Workbench 2019, then I think you should try to start modeling all over again by following the steps shown in the video, and you suppose to get the proper results eventually. If you use a newer version, also try the steps explained in the pinned comments.

The warning can be ignored, it won't affect anything. I never verified this beam with WB2021, so what I am about to say below is my guess of what you should try. Suppress the SOLID65 APDL command while still keeping CEINTF APDL command active. By doing so, your FEM is now linear and should be ready for linear analysis. If the problem still persists, then I don't think there is anything to do with the ANSYS version.

@@ThanaponBuamongkolChannel Thanks for answering. When I did that, it converged, but I need a non-linear analysis. I have a double-span beam with 3 supports and 2 impactors. My supports and impactors don't have a line in the middle so I can't put edges in displacements, instead I put faces if that's okay. Maybe it has something to do with rigid body movement?

The concrete material model in this tutorial will neither work with unloading behavior nor cyclic behavior. To be specific, the "MELAS" APDL command is where the limitation comes from.

@@ThanaponBuamongkolChannel Thank you very much for your reply. Dear Dr. If you do not mind, could you upload a video related with my question? And I want read your papers to study more. Could you share your paper DOI?

In the past, ANSYS Mechanical APDL allows concrete strength degradation and unloading/cyclic behavior. But I never test them in Workbench, not yet.

@@ThanaponBuamongkolChannel Thank you very much. I will study about that.

The solution refuses to run at all or running but just not converging? Please try the following, see if it could help you pass the error. After you have followed every step and the model refuse to run, try to recheck all the rebars are set to "Link" instead of "Beam" and also meshing element order shall be set to "Linear". Named Selection is also a critical part as it directly tied to the APDL command. The element grouped in the Named Selections and its name needs to be exactly the same as shown in the video for APDL command to properly working. Although meshing size and substep size can vary, it is recommended to follow the exact same meshing size/substep size as shown in the video for your first run. Once you succeed with your first run and get the complete results, you can play with meshing size/substep size later on in combination with restart analysis to continue the solution after failing the convergence. After trying all the above, if the model still does not run may be better to restart from scratch and follow the steps again in case something has been previously overlooked.

Thanapon Buamongkol no the solution runs. But it doesn’t converge. And substeps converge is not displayed in force convergence curve.

In case you have restarted and followed every step all over again and solutions still not converging. Skip this tutorial and try another one (RC Column) here in this link below, this one is the easiest to converge among all of my tutorials. kzfaq.info/get/bejne/iK55ZMmmrqesd6c.html Once you succeed with the RC column, you might be able to figure out what went wrong with your RC Beam.

@@ThanaponBuamongkolChannel I was able to converge the solution with out any error and some result matches with your result but the top 10mm rebars are not meshed and are not showing any bonded behavior for BS 7. If I send the project file can you help me in identifying the error?

Try to make sure that the line geometry is not suppressed. Then update the mesh (right-click at the "Mesh" sub-menu then click "Generate Mesh") and check if you can see the meshing (hiding other geometry will also help.)

If your project involves the perfect bonding between concrete and rebar (by assuming rebar never slipped), then there should be no problem analyzing reinforced concrete structure regardless of rebar orientation. The perfect concrete-rebar bonding assumption is common according to ACI-318.

@@ThanaponBuamongkolChannel based on your video sir. You imported the rebars. Is it not possible to model diagonal rebars within the ansys software? We've only seen tutorials but all of them were non-diagonal rebars. And your tutorial is the only one we've seen with a diagonal, but it was imported.

@@kennethmilleza2989 You can definitely model any rebar shape in ANSYS without any other software. Check out Spaceclaim or Mechanical APDL for more information on which one suits your need.