November 6, 2018 at 7:32 pmlrahimiSubscriber
I'm trying to simulate a welded axle design in ANSYS Static structural. I want to find the crack location around the welding connection while forces are applied. Every fracture mechanics tutorial is for the case with the known crack initiation location. Here my aim is to find that location which the crack starts happening from. Can anyone guide?
November 6, 2018 at 7:36 pmlrahimiSubscriber
November 6, 2018 at 10:01 pmpeteroznewmanSubscriber
Cracks grow from flaws in the weld at the location that sees the highest tensile stress amplitude. Cracks don't grow where the stress is compressive. Cracks don't grow if there is no cycling from high stress to low stress.
Use a Maximum Principal Stress plot to show the location on your model where the maximum value of tensile stress is. I imagine you have a Static Structural model. Duplicate the model and put the opposite or negative load on the model and look at the same location to see what the minimum principal stress is. The difference between those two numbers is the stress range.
Please post some screen snapshots of the location with the highest tensile stress range.
November 7, 2018 at 3:41 am
November 7, 2018 at 2:31 pmlrahimiSubscriber
Thank you for the explanation. For the duplicate model that you said I should put the opposite loads on, should I find the stress range for the locations that had maximum tensile stress? What should I do with the stress range after that?
I have an original report where someone else showing the crack locations by doing fatigue analysis. In that report there was contours of fatigue margin, fatigue sigma dyn and fatigue sigma mean. Do you know what those plots are?
November 7, 2018 at 2:31 pmlrahimiSubscriber
Thanks you Sandeep. I'll go through the materials and see if I can learn more.
November 7, 2018 at 2:43 pmlrahimiSubscriber
Should I keep the location of the support and only make the loads negative? I don't see why I should do this.I would appreciate it if you explain the whole process.
November 7, 2018 at 2:54 pm
November 7, 2018 at 3:41 pmpeteroznewmanSubscriber
Please show the supports and the loads on this model. Describe how the load changes during operation of that part in the machine.
I can imagine two different machines. Machine "Z" uses that round bar to support a weight at its end, and that weight is applied and removed. Therefore the stress range is from zero to the value you show. There is no need to duplicate the model in this case. If the weight is never removed, then there is no fatigue possible unless there is some vibration.
Machine "R" uses that round bar to support a force that goes to the right and then reverses and goes to the left. If the image above is for the force going to the right, you would duplicate the model and make the force go to the left. Look at the location on the weld where the maximum of the Maximum Principal Stress was found in the force-to-the-right model and measure at that same location the minimum of the Minimum Principal Stress in the force-to-the-left model. The difference between those two values at that point is the stress range.
You would use the stress range to look up the fatigue life for that stress range on an S-N curve for welds.
The Standard also provides data on variation around the mean. Here are the 2-sigma curves.
The standard includes the equations and coefficients if you want to put the Stress-Life data into ANSYS and have the Fatigue Tool compute the life for you on every point in the model.
If you put the report you mention into a zip file, you can attach the zip file to your reply.
November 7, 2018 at 4:48 pmlrahimiSubscriber
Unfortunately I can not provide that report for some reasons.
So The way the loads are is that there is a downward force as shown in the following picture. And then there are two downward forces applied to the surface at the end of round bar (on both sides). This second force is cyclic. It can be present or not depending on the performance of the machine.
November 7, 2018 at 4:58 pmlrahimiSubscriber
From what you said, I assume that the stress changes from a positive tensile stress to a larger value and the range is the difference. Is that correct? And the range should be sought in the standard plots?
What is the difference between the two plots you attached? 50% failure and 2.3% failure. I don't see a difference in there. Also I think you missed my question about the sigma mean and sigma dyn contour plots.
Here is a section of the contour plot for the sigma dyn in the report I mentioned.
November 7, 2018 at 6:30 pmlrahimiSubscriber
Is there an email address I can connect to? I'm a little in shortage of time until I can get my simulations to a final result.
November 7, 2018 at 7:50 pmlrahimiSubscriber
In order to do the fatigue test can I use fatigue tool in static structural?
November 7, 2018 at 9:41 pmpeteroznewmanSubscriber
I check my email less frequently than I do this site. If you want to reply with your phone number, I can call you, but know that this is a public website and Google is indexing it constantly.
"the stress changes from a positive tensile stress to a larger value and the range is the difference", that is correct.
"the range should be sought in the standard plots", yes.
"What is the difference between the two plots you attached? 50% failure and 2.3% failure. I don't see a difference in there." Look at a specific life of say 2 million cycles. On the 50% plot for the W weld, the stress range is 58 MPa, while on the 2.3% plot for the W weld the stress range is 42 MPa.
"I think you missed my question about the sigma mean and sigma dyn contour plots." I didn't miss the question, I asked for the report. When you say "I can not provide that report" do you mean you are not allowed to, or that you are having difficultly attaching the report to your post? If the latter, put it in a zip file and attach the zip file. Sdyn is not a familiar term to me. What software made that plot?
ANSYS allows you to enter the S-N curve into the material defined in Engineering Data. The Fatigue Tool can take a Static Structural result and plot the life as a function of the stress in the solution, by looking up the life on the curve. You tell the Fatigue Tool if the alternating stress is reversed, zero-based, or a percentage of the load. The last one would be your category.
November 7, 2018 at 10:09 pmlrahimiSubscriber
Thank you Peter. I am not allowed to share that report.That's the problem.
Now I understand the difference of the two plots you shared and thank you for that.
So I have these questions now:
1:Now that I have the standard S-N should I use the lower failure rate (2.3% for example) to make sure the weld cracking is less probable?
2: If these are stress range (S_max-S_min) Do we have mean stress values (S_max - S_min)/2+S_Min plots, constant life diagrams?
3: I still have difficulty giving the fatigue tool a ratio value. I think the ratio of the stress change differs depending on the location.
November 7, 2018 at 10:14 pmlrahimiSubscriber
Maybe the sdyn plot is the alternating stress plot! But then I don't see an option for the sigma mean plots! I don't know the software they used. I have limited information about the report that I'm supposed to replicate its results!
November 7, 2018 at 10:24 pmpeteroznewmanSubscriber
1. It's up to you if you use the 50% failure probability and a large factor of safety or the 2.3% failure probability and a small factor of safety. In either case you need a factor of safety. I like to use the 2.3% curve, but it is not commonly made available. The 50% curve is typically provided for most materials.
2. Yes, you have a mean stress and the ANSYS Fatigue Tool can include a Mean Stress Theory.
If Analysis Type is set to Stress Life, choose from None (default), Goodman, Soderberg, Gerber, ASME Elliptical, and Mean Stress Curves. The Goodman, Soderberg, Gerber, and ASME Elliptical options use static material properties along with S-N data to account for any mean stress while Mean Stress Curves use experimental fatigue data to account for mean stress. You can specify the default setting for this property using the Mechanical application Fatigue settings in the Options dialog box.
3. If the high and low loads do not create what is called Proportional Loading, then you can use Nonproportional Loading in the Fatigue Tool and have exactly two Stress Results to put into the tool.
The options of the Type property are described below. Their availability is based upon your analysis type.
Fully Reversed (r=-1)
Non-proportional Loading (available only for stress-life applications)
The Zero-Based (r=0), Fully Reversed (r=-1), and Ratio options are all constant amplitude, proportional loading types and are graphically illustrated in the Worksheet.
The History Data option enables you to import a file containing the data points. This option is a non-constant amplitude proportional loading type. This data is depicted in a graph on the Worksheet. You can specify the number of data points this graph will display using the Maximum Data Points To Plot property in the Options category.
The Non-proportional Loading option is a non-proportional constant amplitude loading type for models that alternate between two different stress states (for example, between bending and torsional loading). Problems such as an alternating stress imposed on a static stress can be modeled with this feature. Non-proportional loading is only supported for Fatigue Tool objects in a Solution Combination where exactly two environments are selected.
You should read the entire ANSYS Help file on the Fatigue Tool.
November 8, 2018 at 6:27 pmlrahimiSubscriber
Thank you so much for your explanations. One more question, Should I add weld S-N curve information to the engineering data sheet or they are already there? Should I have an assembly design and do weld connection in ANSYS simulation. I mean how do I tell the software that the connection is welding and it should use the welding curve for that region?
November 8, 2018 at 6:37 pmpeteroznewmanSubscriber
To create a weld bead as a separate body, simply revolve a triangular cross-section around the pipe where it is welded onto the plate. Use bonded contacts to connect the weld bead to the pipe and the plate.
In Engineering Data, create a weld material and add the weld S-N curve to that material, along with Isotropic Elasticity.
November 8, 2018 at 7:58 pmlrahimiSubscriber
So where do I find the weld material S-N to add to the engineering data? Should I enter it manually?
November 8, 2018 at 9:01 pmpeteroznewmanSubscriber
I provided the table for the 2.3% Failure probability for the type W joint in the post above. You can enter that manually.
November 8, 2018 at 9:03 pmlrahimiSubscriber
I saw that peter. Thanks. Just wanted to make sure if it's already there or not. And I should use the structural steel for other properties, right?
November 9, 2018 at 1:22 ampeteroznewmanSubscriber
You should create a material that matches the material specifications for the parts in your assembly. Different steels have different S-N curves, but you will find that the weld has lower fatigue life than any parent steel, so it doesn't really matter. You can use Structural Steel.
November 9, 2018 at 6:19 pmlrahimiSubscriber
Do you you why my mesh connection group is deactivated? I can not have connected mesh between parts.
November 9, 2018 at 8:50 pmlrahimiSubscriber
Do you know why I can not do mesh connection?
November 9, 2018 at 10:39 pmpeteroznewmanSubscriber
Please show a screen snapshot of your geometry, including the Geometry branch in the outline, expanded so I can see how many bodies there are, and the mesh connection group. Maybe it is deactivated because you only have one body?
November 12, 2018 at 2:25 pm
November 12, 2018 at 2:27 pmlrahimiSubscriber
After you told me about how to build the weld bead I designed it in separate parts to be able to separate the weld and round bar from the rest of the body.
Still it does not let me connect their mesh elements. I don't know why this option in not activated.
November 12, 2018 at 2:28 pm
November 12, 2018 at 3:18 pmlrahimiSubscriber
I added shared topology in geometry and it is connecting mesh elements automatically now. I don't know what is the use of Mesh connection if I could have a shared topology do that for me. Maybe it's used for body-surface connections.
November 12, 2018 at 4:33 pmpeteroznewmanSubscriber
Mesh connection is useful if the geometry came straight from a CAD interface and did not come through DesignModeler or SpaceClaim. You can set shared topology in DM and SC, but not in any other CAD system.
November 12, 2018 at 7:14 pmlrahimiSubscriber
What if I needed the information on the connection planes or I needed to change the connection from bonded to something else? Shared topology does not let me create connections.
November 13, 2018 at 12:22 ampeteroznewmanSubscriber
If you need information at the interface between two bodies, then use bonded contact and don't use shared topology. It's great to have options!
November 13, 2018 at 9:29 pmlrahimiSubscriber
If I don't use shared topology it wont connect the mesh!
Also, can you guide me if my load application cycle has more than 2 stages, what can I use instead of Non-proportional type?
For example if I have a cycle of 7 steps of load application, how can I do fatigue analysis on the model?
November 14, 2018 at 1:07 ampeteroznewmanSubscriber
I don't understand what you mean when you say "If I don't use shared topology it won't connect the mesh!" You define Bonded Contact between the faces that are coincident. Each face has its own mesh. The mesh is not connected. Bonded Contact creates elements to connect the two faces. You don't see the elements in Mechanical, but they are created by the solver. If you choose type MPC, you can see the elements after the solver has finished.
November 14, 2018 at 2:47 pmlrahimiSubscriber
So I believe I should be able to use mesh connection group to connect the mesh on the edges of two bonded faces., right? (And probably the faces themselves. When I use shared topology the contact faces are considered one and I can not distinguish them and when I don't use the shared topology the software deactivated mesh connection group so the mesh is not conformable anymore!
November 14, 2018 at 7:58 pmpeteroznewmanSubscriber
What version of ANSYS are you using? You are in Workbench, not AIM, right?
Please reply with inline images of the screen snapshots saved that show the Outline window fully expanded and the geometry window for the case when Shared Topology is not used.
You can attach a Workbench Project Archive and I will download that and see if I can determine what is wrong.
- You must be logged in to reply to this topic.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- Saving & sharing of Working project files in .wbpz format
- An Unknown error occurred during solution. Check the Solver Output…..
- Understanding Force Convergence Solution Output
- Solver Pivot Warning in Beam Element Model
- Colors and Mesh Display
- How to calculate the residual stress on a coating by Vickers indentation?
- whether have the difference between using contact and target bodies
- What is the difference between bonded contact region and fixed joint
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- User manual
© 2023 Copyright ANSYS, Inc. All rights reserved.