Mesh, design issues for SC static structural

  • 126 Views
  • Last Post 26 December 2018
  • Topic Is Solved
jackhero posted this 18 December 2018

I designed a geometry (shown below) in Ansys spaceclaim for static structural analysis based on a previous discussion, I would like to request guidance on the following issues,

Although some part of the reinforcements are protruding outside (I should have fine tuned the geometry to keep them inside), I just ran the simulation to check for any possible issue(s). Hope that the following issues are not due to this protruding problem.

1. In Mechanical, I got a weird mesh for the reinforcements (shown below in the first image). The mesh looked ok for the block (shown below in the second image along with the reinforcements). Please note that there was not any modification done for the mesh, so the following images are for the default mesh size or settings.

(2). I followed another discussion on adding same element to several geometries and added the code mentioned there, for converting beam to link180. I would like to ask that;

(2-i) With in the code, the area is mentioned as (area = 3.1414), this area is also mentioned for the beam reinforcement which I designed in SC,

The beam diameter I would like to use if 0.035mm (radius of 0.0175mm). How can I change the default diameter size to my desired one? If I am not mistaking this was also mentioned by Peter in one of his reply to question number 3b, but we couldn't discuss on editing it. Please note that the number of reinforcements are in hundreds or thousands, a general way of assigning/setting the diameter would be useful.

(3). How can I add contact between concrete and the reinforcements? Ansys doesn't automatically detects the contact, I tried manually creating the contact but the reinforcements are not detected/included by the contact wizard. I could only select the block for target and contact body. I tried hiding the block and then manually dragging and selecting all of the reinforcements but it didn't work. Also, I creating named selections for both but it didn't work either.

 

(4). One question regarding Spaceclaim (SC) I would like to add. Suppose if I am working in static structural and while designing geometries in the Design Modeller (DM), after I finish designing and close the DM, the geometry is automatically detected for the subsequent steps (like Model, Setup, Solution...). But if I finish designing geometry in SC and I close it the designed geometry is not detected by the subsequent steps. Any suggestion for this issue? As a temporary workaround, after finishing the designed geometry in SC I save the file and then import the geometry in Static Structural.

 

(5). For the trial run of the above model, I set the boundary conditions as the following,

Although, in some discussions the usage of displacement at the bottom is suggested instead of the fixed supports, but for the trial run I ran the simulation, which as per my understanding given the current boundary conditions, shall bring some results. But I had the following error.

A solver pivot warning or error has been detected in the UX degree of freedom of node 7206 located in Design2\Beam (Circle). This is usually a result of an ill conditioned matrix possibly due to unreasonable material properties, an under constrained model, or contact related issues.  Check results carefully. You may select the offending object and/or geometry via RMB on this warning in the Messages window.

 

  • Liked by
  • Mirghani
Order By: Standard | Newest | Votes
peteroznewman posted this 18 December 2018

Hello Jack,

(1) The line bodies have a circular cross-section with a 10 mm radius as defined in (2-i). Look at Jason's code for assigning section properties to the LINK180 elements.  Note that area = 3.1414 is in square mm if your unit system is currently in mm, or it is in square inches if you unit system is in inches.  Once you pick a unit system to insert a command object, you must Solve with that unit system.  For your radius of 0.0175 mm, you would set area = 9.6211e-4 with the units set at mm.

(5)  One way to test if all your reinforcements are connected to the concrete is to run a Modal Analysis. If you get any zero frequency results, you have at least one loose fiber. Just drag a Modal system from the toolbox onto your model cell, then drag and drop the two Fixed Supports onto Modal in the Outline, then RMB on Modal and Solve.

I will post now and hope some other members can answer some of your other questions.

Regards,
Peter

  • Liked by
  • jackhero
  • Mirghani
jackhero posted this 19 December 2018

Thank you for your reply.

I ran the Modal Analysis and I got zero frequency. The images are shown below. Could you please guide me on how shall I connect all reinforcements to the concrete block?

Also, could the mesh problem which I mentioned above be related with the un-connected geometries of both reinforcements and the block? And is there any alternate way of generating the mesh on the reinforcements?

peteroznewman posted this 19 December 2018

Jack, 

The only way I know to connect reinforcement line bodies to solid elements in Static Structural is by node-to-node connections using Shared Topology. Do you know how to use that?

In Explicit Dynamics, it's a different story. The elements can "grab onto" the reinforcements without having to share nodes.

I hope someone else can describe another option.

Regards,
Peter

 

jackhero posted this 20 December 2018

Firstly I designed the block in spaceclaim (SC), then under properties I set the Share Topology to 'Merge' then I imported the reinforcements and converted them into beam (shown below in the first image). With this geometry I re-ran the Modal Analysis and I again had the zero frequency (shown below in the image). Is there anything I missed for the Share Topology?

Please note that I also tried setting the Share Topology to 'Share' instead of 'Merge' but still getting the zero frequency with it.

 

peteroznewman posted this 21 December 2018

Jack,

Setting Shared Topology in SpaceClaim 18.2 to Share does not cause the solid mesh to share nodes with the beam element mesh.

It didn't help going into the Workbench tab and using SharePrep and Share.

I suggest you ask some of the other members who have been building reinforced concrete models.

Regards,
Peter

 

  • Liked by
  • jackhero
jackhero posted this 22 December 2018

I think I also have some issues either with SC or its settings. I created two geometries in SC (here) one with Shared Topology (design4 in attachment) and other with Merged topology (design5 in attachment). Apart from the issue which I mentioned in my first post (question#4), I get the following error when I open the Shared topology geometry (design4) in Mechanical,

Unable to attach geometry. Plug-in Error. The geometry editor was closed abnormally (this error I get everytime when I open or deal with SC. After I click Ok on this message SC does open though).

I searched for solving on these errors and also did the CAD configuration Manager Modification (as an admin) but it didn't help. I also tried saving the SC geometry in *.igs format but it also did not work. Any suggestion on this issue would be helpful.

However, I did not have any issue when I opened the Merged Topology geometry (design5). But when I mesh the geometry I had the strange mesh which I mentioned in my first post. Could you please check both of the geometries to see if you are also having the same issues as me, one on SC errors and other on the strange mesh design (as shown in my first post) in mechanical?

I tried checking the geometries in DM. If I opened the DM and then imported the geometry (either Design4.scdoc or Design5.scdoc) and generate I only had the solid block without any reinforcements. As a workaround, I under Project Schematics, after dragging the static structural, I right-clicked on Geometry and then import the SC file (*.scdoc). Then right-clicked on Geometry again and select Edit Geometry in DM. After loading the DM, I clicked on generate and this time I had the reinforcements as well. But I had the cross-section error in DM for all of the Beam(Circle).

Could you please guide me on assigning the cross-section in DM properly? As a temporary workaround I selected all of the Beams and formed new part. That cross-section issue was gone temporarily in DM with this step. I then opened the geometry in Mechanical and again had the question mark for all of the beams with the same cross-section issue.



I proceeded with the mesh and the mesh for the edited version of the SC geometry looked different (but maybe not perfect) than the SC mesh (which I posted in my first post). I couldn't run the Modal Analysis on this due to the cross-section error.



peteroznewman posted this 23 December 2018

Jack,

Please read the ANSYS help file, Chapter 14: REINFORCING which seems to have what you want.

14.3.1. Mesh-Independent Method

The mesh-independent method offers much flexibility when the base elements are arbitrary and have no distinct patterns for the reinforcing to attach.

The reinforcing location is represented via a mesh with MESH200 elements. Other model information, including reinforcing material, cross-section area, spacing, and orientation, can be provided via by a reinforcing element (REINFnnn) section (SECDATA) or MESH200 element data.

MESH200 elements can be combined with base elements and reinforcing sections in various ways:

Using the Mesh-Independent Method:

  1. Create the base elements.

  2. Create MESH200 elements with appropriate reinforcing (REINFnnn) sections.

  3. Select the base elements and the MESH200 elements.

  4. Generate the reinforcing elements (EREINF).

  5. Inspect and verify the newly created reinforcing elements.

As shown in the following example input listings, you can manually adjust the translucency of the base elements to show the reinforcing elements. Additional automatic reinforcing display options are available via the GUI (Main Menu> Preprocessor> Sections> Reinforcing> Display Options). 

Regards,
Peter

  • Liked by
  • jackhero
jackhero posted this 26 December 2018

Thank you for the guidance to the ANSYS manual for reinforcements section. After going through the manual if have any query regarding the suggested reinforcement section I will post a separate discussion.

With reference to your post within this discussion, in which you posted the image of shared nodes. I would like to ask a general query that I am interested in getting an image as following (for my another contact model), which as per my understanding is related/similar to the one which you posted above.

I searched for it but I could only find ways of doing it in APDL. Is it possible to get such image(s) for any contact model (having contact and target elements) in Ansys workbench? Although in the attached image Gauss integration is mentioned but I used program controlled for my model.

peteroznewman posted this 26 December 2018

Workbench uses the Mechanical app to build a model, but at the end of the model building process, when you click Solve, Mechanical is writing out APDL code to submit to the solver.  So anything to do with how the solver computes contact is going to be in the APDL section of the ANSYS Help system.  There is only that entry, there is no separate entry in the Workbench Mechanical Help. I hope this answers your question.

 

Close