Learning Forum

[Isshaan]

Hello.

I'm new to this simulation World and tried simulating the Dye for Deep Drawing process. 

I've created a setup, but it shows certain errors and the result could not be converged. 

Attached is the project file. Can someone please help me with the same?

[peteroznewman]

Without looking at your setup, I can recommend you study this discussion.

If you need help after studying that, reply with details on what is going wrong in your simulation.

[Isshaan]

 Hey. Thanks for replying. I just had a look at the discussion you shared, but I would still prefer doing it in 3D. Can you please take a look at the attached file and help me out?

Please make corrections and explain them as well, if you can.

Thank You

[Isshaan]

Ya, One more thing, Can you also suggest some tutorials for learning Ansys?

[peteroznewman]

You will learn many useful things building a punch and die in 2D that will directly apply to a 3D simulation.

Here is a Tutorial on how to create an Axisymmetric Model. Similar approach is for a 2D Plane Strain model.

I will be happy to help solve any issues with a 2D model. Once that is working, then we can look at 3D.

[Isshaan]

Thanks for the response. 

Can you please share your E-mail ID?

or, Can I contact you Directly over some Social Platform?

[peteroznewman]

This is it.

[Isshaan]

 Hey, I tried doing the same way. But is shows the following notification. 

[Isshaan]

Can you please once solve this problem and provide me with the solution? So that 

I can have a look at how the things were done? 

[peteroznewman]

The surfaces under the Geometry window has ? on them. Click on one and see what is missing, the Material assignment or the Thickness.

Also, you can't take a 3D model had a Mechanical model built and change the Geometry to 2D and reuse the Mechanical model. That doesn't work.

I suggest you create 2D geometry with and start a new Static Structural.

[Isshaan]

I've opened a new project. In SpaceClaim, created this view of the desired simulation body, used pull tool, to define a thickness of 1mm. But, it would then be considered as a body. So, just added a surface. 

[Isshaan]

Plus, in the model section, it should detect 3 surfaces, but it's only taking 2. The bottom one and the plate (the centre one) are in one single part.

[peteroznewman]

1) When using the Pull Tool, the default is Merge so that can take 3 bodies and turn them into 1 body, which is not useful. Make sure to change the Pull tool to No Merge before you pull on them.

2) These surfaces are in the XZ plane. The must be in the XY plane. Use the Move tool to rotate all surfaces 90 degrees into the XY plane. Again, the Move tool has Merge as the default. You don't want to collapse 3 surfaces down to 1.

3) To get started, take just one rib in the pattern to learn the simulation. The solution will run much faster if you slice away most of the geometry.

[Isshaan]

I tried the same. But as soon as I select the pull tool, it automatically selects 3 faces and gives them Surface under Single Surface. I can't get this, how to settle this. 

[Isshaan]

I can see 3 Surfaces in SpaceClaim but as I open Model, it loads only 2.
The Lower One is Merged with the Middle One.

[peteroznewman]

Start over. Create three components. Activate one component and make one surface, then activate the next component for the next surface and repeat one more time. The Pull tool cannot merge geometry from another component.

[Isshaan]

 

This is what I can see after the model settings. 

[Isshaan]

Okay, Solved this. 

Attached is the file. Please have a Look. 

[Isshaan]

Hey @peteroznewman. 

[peteroznewman]

There is a lot wrong in the B system. I will point out a few items you need to fix.

1) In Workbench, the Geometry cell Property row 12, Analysis Type is not set to 2D, it is set to 3D. That means you have to start over on Static Structural. Use the Geometry from that file, but set the property to 2D on a new Static Structural.  You can't fix this one.

2) In Mechanical, you set the deformable body to Rigid. Leave it flexible.

3) I recommend you do one hump not six as your first model.

 

[Isshaan]

And about other things/settings in model?

 

[Isshaan]

I've followed your instructions and did the same in a new project.

The file is attached and please help me out further. I wanna know and learn this simulation thing. 

[peteroznewman]

Isshaan, please follow the example I provided more closely.

Did I not show that you need 4 elements through the thickness of the sample?  Your model only has 1 element.

Did I not advise to put a radius on the corner of the bottom die? Your model has sharp corners.

Did I not advise to turn on Auto Time Stepping and set the Initial Substeps? Your model has Program Controlled.

[Isshaan]

 

When I'm generating the mesh, The mesh only appears on the workpiece and the edges of die and punch, and not on the complete face of die and punch, as in the image of the example. 

[peteroznewman]

Your model is using Rigid bodies for the punch and die so the mesh only appears on the surfaces that have contact defined. That is fine.

Does the mesh on the workpiece have 4 elements through the thickness?  You can apply Face Meshing to the surface and Edge Sizing to the two short edges to set them to have 4 elements.

[Isshaan]

Yea it does have 4 elements.

 

And these are the errors I'm facing. 

[peteroznewman]

Please show the Details on the Analysis Settings. I think you missed something.

Do you see how the elements get skewed in the mesh. Add edge sizing to the long edges of the workpiece to force the elements to remain square along the length.

[Isshaan]

I can't get perfect squares in mesh. 

 

Here is the analysis settings. 

 

[peteroznewman]

For the Mesh Sizing controls, change the behavior from Soft to Hard

Follow the directions in this post.

[Isshaan]

 

 

 

Sir, I followed your mentioned post, but I couldn't understand the points mentioned in it completely. 

[peteroznewman]

Click on the Solution Information folder, on the Solution Output line, pull down the menu and select Force Convergence. Insert a screen snapshot of the plot that shows.  Now expand the + on the Solution Information folder and there will be three plots. Click on each one. Insert a screen snapshot of one of them.

[Isshaan]

[peteroznewman]

The N-R Force Residual Plots are only useful if you turn on the Maximum flag and zoom in until you can see the element where the Maximum flag is.

It is also easier to converge if you slice the model in half, that way there is a constraint on the X displacement of the material at the center.

[Isshaan]

Slicing the model along Y-axis?

[peteroznewman]

Yes, exactly, and adding the X=0 Displacement boundary condition on the short cut edge of the sample. The rigid bodies don't need to be sliced in two, only the workpiece.

[Isshaan]

When I insert the symmetry region and select the 3 rightmost edges, there's a question mark on the symmetry tab. 

[Isshaan]

Tried again. Same error.

 

[peteroznewman]

Click the Maximum button.  Fit the view until you can see where the Maximum flag is. Zoom in on the elements around the Maximum Flag. Make a screen snapshot of that area.

[Isshaan]

[peteroznewman]

Please show a screen shot of the contact details on this interface.

[Isshaan]

[peteroznewman]

Why are there two edges in the Contact definition?  If the 2 edges are the top and bottom edges of the workpiece, that is a mistake. There should only be the edge on the top of the workpiece for the top contact and the single edge on the bottom of the workpiece for the bottom contact.  

[Isshaan]

You told to slice the workpiece along y-axis. That's why there're two edges.

I'll attach the file, you may please have a look. 

[Isshaan]

Sir, Please?

[peteroznewman]

I will take a look today.  Since there are so many ways to fail, I have to ask about each idea I have that would cause it to fail. I can't see exactly what you did until now.

[peteroznewman]

This was a very difficult model to achieve convergence. One reason is how long and thin the workpiece is compared with the example where it happened easily. I recommend you change this to an Explicit Dynamics model. That has no problem with convergence.

Note that if you move the die back up to the starting position, the workpiece will straighten out. That is because you have no plasticity in the material model.

This discussion has become too long. Please mark this post with Is Solution to mark the discussion as Solved and open a New Discussion for any followup questions. You can insert a link to this discussion in the New Discussion.

[dominic t]

@peteroznewman

 hi, there I'm working on a non-linear analysis of reinforced concrete beam and i need to model two beams with M20 grade and M25 grade concrete and the rebar diameter needs be changed in each beam.

I'm using Solid65 and link180 element for modelling, i used the solid65 with M20 grade concrete properties and it worked and later when i changed the command for M25 grade concrete its executing the command but the results are same as that of M20 grade concrete. In case of link180 element i want to change the diameter of the bar and im not able do that.

can you please help me out

[Nanda]

Hello dominic,

I suggest you open a new discussion, if you feel your query is closely related to this topic, kindly share the link of this discussion along with detailed description of your issue

Regards,

Nanda.

Guidelines for Posting on Ansys Learning Forum

How to access ANSYS help links