Learning Forum

[sagar.gupta.satrasala]

Hi,

I am trying to split a geomtry(cyclindrical body) into 3 parts and assign different material properties for each layer for my project. Can someone please help me with this issue.

The left image is the geometry i created and the right side image is how I want to my geometry to be in 3 layers.

 

 

[peteroznewman]

Open SpaceClaim, File Save and name it 3layers.scdoc.  Create a New Component and name it Layer1. Sketch two circles and Pull the solid cylinder.

Activate the parent file called 3layers, create a New Component and name it Layer2. Sketch two circles and Pull the solid cylinder.

Activate the parent file called 3layers, create a New Component and name it Layer3. Sketch two circles and Pull the solid cylinder.

Activate the parent file called 3layers, click on the Workbench tab and click the Share button.

Now you have three solids that will share nodes at the two common surfaces. In Mechanical, each solid can be given a unique material.

[sagar.gupta.satrasala]

It worked.Thank you so much for your help!!!!

[sagar.gupta.satrasala]

Hi,

Could you please help me with one more error that I am facing,

I created 3 solids and now I have to create a solid intersecting these 3 solids, I couldnt do that properly in spaceclaim so I did it in designmodeller.

I have attached a picture of that below:

Everthing is fine after I created it, but there is a error warning message that says,

Warning: Extent surface intersects one or more profiles. Unexpected result may occur. Context: Extrude Feature Extrude1

Could you please tell me what this error means and what I should do to correct it.

Thank you!!!

[peteroznewman]

It's a warning, not an error.

What is the goal of this new solid?  Is it supposed to be another material? In that case, it must replace the solids that currenly occupy that space. Create a plane on each face of the new solid and use those planes to Slice the three solids of the pipe and delete the intersection solids.

[sagar.gupta.satrasala]

I am trying to design 3d model of bamboo to conduct stability analysis on them.

This new solid is a diaphragm inside the bamboo and it is present at each node(which has same distance between them all over the bamboo).

The model kind of looks like this

[peteroznewman]

Okay, then the diaphram should have an OD that is equal to the ID of the inner cylinder so there is no overlap. Then use the plane on each side of the diaphram to slide the cylinders. In DesignModeler, put all the solid bodies into a single part by selecting them in the outline then right click and select Form New Part.  This will create Shared Topology and the mesh on each solid will be connected to its neighbors by sharing nodes.  You can also try to use a Linear Pattern to replicate the structure from the first copy down the line.

[sagar.gupta.satrasala]

Hi,

I designed the diaphram with an OD that is equal to the ID of the inner cylinder, but I am still getting the warning

 

[peteroznewman]

Use the Workbench File, Archive and save a .wbpz file and put that on a File Sharing site such as Google Drive, OneDrive, Dropbox or Jumpshare.  Put the link to the file in your reply.  Also say what version of Ansys you are using.

[sagar.gupta.satrasala]

I am sharingt the one drive link of the file below,

https://1drv.ms/u/s!Ak6OQiAK1pPQjy1d5XHRlp7r-3NS?e=skbSXg

Thank you so much for taking the time to look at this!!

[peteroznewman]

Please reread my previous reply and follow the directions exactly. You uploaded a *.wbpj file, which is useless without the matching *_files folder. This is what the Archive does, it creates a .wbpz file that includes the folder.

Also, you did not say what version of Ansys you are using. If you are using Ansys 2021 R1 and I open your file in Ansys 2022 R2, you will not be able to open the file I send back to you with the changes I made.

[sagar.gupta.satrasala]

Hi,

I am sorry about that. I am sending you a link of a zip file with the .wbpj file and the files folder in it. I am using Ansys 2022 version.

https://1drv.ms/u/s!Ak6OQiAK1pPQkjT4gbT0o2bnLn8V?e=Vbltbw

 

[peteroznewman]

You didn’t use Form New Part correctly in DesignModeler so you have a lot of contacts and the mesh doesn’t line up.

Right click on Diaphragm and Explode the Part, then select all the bodies and Form New Part.

Now there is no contacts and the mesh is connected.  I also reduced the element size to 25 mm.

If you take the surface of the Diaphragm and extend it out beyond the Layer1 solid, then Slice Layers 1 – 3, you will get hex elements on Layer 3 instead of Tet elements.

I also found that in Mechanical, the Layer 1, 2 and 3 solids were assigned to Structural Steel and not Bamboo L1, 2, or 3. Make sure to check material assignments!

[sagar.gupta.satrasala]

 

Thank you so much for your help and suggestions. 

I tried the creating a new part to put all the solids but still the warning is there. 

Does extending it out beyond the Layer1 solid, then Slicing Layers 1 – 3 take the error out?

 

[peteroznewman]

You will get a better mesh (all Hex elements) if you extend the curved shape of the diaphragm out past the OD of the outer layer and slice all the layers for the top and bottom surface of the diaphragm. Then put all those solid pieces into a single part.

[sagar.gupta.satrasala]

Hi,

I am trying to create an external body on the surface of the outer diameter but I am not able to create a line on the surface of the outer layer. How much ever close I am trying to create its still not on the surafce of the outer layer. Could you please give me a suggestion to perform this.

The outline of the body I am trying to create and how it looks like:

 

Is there also a way to cut the solid surface near the diagarm and create another solid like the picture below,

 

[peteroznewman]

These instructions are for DesignModeler. Sketch a rectangle, but make sure the vertical line is inside the outer surface of the existing outer layer.

Revolve this Sketch, then use a Boolean to Unite this ring to the outer cylinder of the shaft. Finally, select the two edges and add a Blend.

[sagar.gupta.satrasala]

Could you also tell me, if there is a way to cut the solid surface near the diagarm and create another solid like the picture below. Because if thats possible I have to make that solid before the one you suggested now. Sorry, if I am asking too many questions. I am doing a project in my masters and I am a bit new to ansys and your suggestions are really helping me a lot.

I have to make it such that it almost looks like this at the diaphragm part, but the person made these in Abaqus not in ansys

 

[peteroznewman]

In your bamboo model, you have Extruded the diaphragm, which makes the connection to the cylindrical part go up and down like a wave. This makes it more difficult to add the nodal ring.  I suggest you Revolve the diaphragm to make the intersection with the outer skin a circle.

This Revolve was Add Frozen.

I then used Concept, Surface from Faces to get the top and bottom faces.  Then I used those faces in a Boolean Subtract from the three solids Layer1, Layer2 and Layer3.

I used Virtual Topology to merge a small face on the node body.

This link is to an ANSYS 2022 R2 archive. https://jmp.sh/WOtJHt4

[sagar.gupta.satrasala]

Thank you for the help. I have created everything as you suggested but I have difficulty understanding the blend part. Could you please explain me how you did that,

I tried doing that but I am not able to create blend on both the sides, if I create it on one side the other side is not showing up.

[peteroznewman]

First blend the edges at the base of the rectangular rib. Make the blend size less than the height of the rib. Second blend the edges at the top of the rectangular rib. Make sure the blend size is less than half the width of the rib.

[sagar.gupta.satrasala]

Thanks it worked, but I am getting an error when i mesh - "The source mesh cannot be correctly copied to the target surface. This might be because the surface is a closed surface with degenerate points. Splitting the surface might help".

Can you also please tell me why you created a ZX plane with an offset of 100mm and split it.

Even in the file you sen, when I mesh I am getting this error

 

[peteroznewman]

Download the file linked to above, open the Model in Mechanical, click Generate Mesh and you will get the same mesh I get unless you change something first.

If you opened the Geometry in DM, then did a Refresh and opened the Model, you may have lost the 4 Faces that were made with Virtual Topology.  Recreate the Virtual Topology and it should mesh again.

I created a ZX plane in DM to cut the length of the bamboo down to a small length so I could mesh and solve the model with the 3 mm element size that gives 2 elements through the thickness of each layer and solve in the Student Limit.

I can change the Element Size to 6 mm and get 1 quadratic element through each layer wall thickness.

[sagar.gupta.satrasala]

No, I didnot refersh in geomter and the 4faces in virtual topoloogy are still there but the error showed up.

I downloaded the file again and I directly opened the mechanical to mesh it and the same errors are still present

[peteroznewman]

The mesher tried to use a sweep mesh method on some sweepable solids and encountered an error in sweeping, so it used the backup tetrahedral mesh method, successfully meshed the sweepable solid and is able to solve the model.  In other words, you can ignore those errors. A workaround was automatically found.

The issue is the node ring is not a sweepable body, so sweepable bodies that touch it can’t be swept after the node ring is meshed. It’s possible with more work to slice the node ring up so that it is sweepable. If you slice all the solids in the XY plane through the diameter, then the node ring is broken into two half rings. Now sweeping could be done on all solids around the axis from 0 to 180 degrees on half the solids and from 180 to 360 on the other half of the solids. Here is what the mesh looks like after recreating the Virtual Topology.

https://jmp.sh/xQcuAWM

[sagar.gupta.satrasala]

Understood. Thank you very much again for your help.

 

[sagar.gupta.satrasala]

Hi,

Is there a way to save my file to older versions, so that I can open it in Ansys 2019. 

[peteroznewman]

No.

[sagar.gupta.satrasala]

Thank you for your reply. My supervisor suggested me to save it as a step file (.stp) and I couldnt find an option for that too.

I have one more problem, I also have to design bamboo with imperfections. One of them is ovality, in this model I am not able to create the outer rectangular part for the diaphram as it is in elliptical shape. I tried extrude also and it doesnt work. Could you please give me a suggestion to model that.

Thank you

[peteroznewman]

The Student license for ANSYS does not provide the ability to save as STEP.

If your supervisor has a Research license for ANSYS, you can send them the Workbench .wbpz archive file. That license can save as STEP, which they can send back to you.

[sagar.gupta.satrasala]

Hi,

Could you please help me with a issue with parameterization. I want to parametrize the diameter of the bamboo in spaceclaim, how to parametrize the 2d sketch dimensions in ansys spaceclaim?

 

[peteroznewman]

I recommend using DesignModeler for parameterization. It is more robust than SpaceClaim because DM is a history based modeler. That means you can always repeat the shape for a given set of inputs.  SpaceClaim has no history so a feature can be consumed during the excursion to one set of values and then that feature is not present when the initial set of values are used again.

[sagar.gupta.satrasala]

I would normally use Designmodelller, but I want to parametrize the diameter, height and thickeness of bamboo which I am designing using Spaceclaim. I parametrized the height as it is in 3D plane, but couldnt do the diameter and thickness of bamboo. I have to do these in spaceclaim as I want three different layers of bamboo and you suggested this way.

[peteroznewman]

You don't have to use SpaceClaim. You can have three different layers of bamboo in DesignModeler, and use Shared Topology, like you have in SpaceClaim, but there is a different method to achieve that.  In DM, when you have 3 Parts and 3 Bodies listed in the Outline, you select the three Bodies, right click and select Form New Part.  Then you will have 1 Part and 3 Bodies, and that is Shared Topology.

[sagar.gupta.satrasala]

Okay. Thank you for the help!!!!!