nCode: Combining Static and Harmonic Results in Fatigue Assessment

nCode: Combining Static and Harmonic Results in Fatigue Assessment Good morning everybody, this is Edwin from Ozen Engineering Inc.

and today we are going to work with nCode and in this video I want to show you how to combine stress results from static structural analysis and harmonic response in the same fatigue evaluation using nCode. Let's start to explain this analysis.

We can see we have two blocks, in this case we have a static structural analysis and a harmonic analysis response which are connected via engineering data, geometry, and model. That means we are going to share the mesh and we will use the same model to calculate both responses.

Let's move to Mechanical and see how those models have been set up. Okay, we have a very simplistic beam here and we have a mesh, not too fine but it's good enough for our purposes. And we have two analyses, we have the static structural and the harmonic response.

In the static structure, we are using a fixed support in the bottom edge and we have a pressure in this load to generate an axial response. Having a uniform pressure, we will expect to see a uniform stress, something similar to a uniaxial stress state.

That won't be exactly the case because we have a fixed support in the end, but that will be close enough. In our second analysis we have the same fixed support but our load in this case will be applied tangentially generating a bending over this body.

Because this is a harmonic load it will oscillate between negative and positive. That means if we apply 15 N here that will be 15 N to the left and to the right, varying sinusoidally during time. and this is how we want to solve the model. Let's solve both analyses and see how the results are.

Ok, we have now the static structural analysis solved and as we expected we see a mostly uniform stress value which is 10 MPa. We can see how the contours have been modified to show the green color band between 9.5 and 10.5 MPa.

That means most of our solid is supporting 10 MPa, which is our intention here. Now, let's solve the harmonic analysis and see the results. Now we can see the normal stress in the vertical direction. We can modify the contour plots to understand how these stresses are developing.

Now, we can see we have a positive value which is close to 25 MPa and the negative side which is minus 25 MPa. This is what we expected because this is a pure bending load. Knowing that, we can continue in Workbench in order to set up our fatigue analysis to combine these two loads.

Okay, being in Workbench, I am going to add a new analysis type here in the toolbox. I can see we have several options from nCode. In this case, to combine these two analysis types I will need to use the swept sine model. I am going to drag it and connect it to the static structural one.

We can see how highlighting all those cells we can use the engineering data geometry model and solution files which is important because we need the results here.

Then I need to connect my harmonic response to the nCode block 2. That will be done just by dragging the solution from the solution to the solution in nCode. Now we can see we have two pink lines which connect from static structural and from harmonic analysis to nCode.

Then we can refresh to update this data into the nCode block. Now, by double-clicking I can open the nCode block. And that will open the nCode interface, which is the Glyph classical interface we all know. We can see this can be overwhelming. This is a bunch of different glyphs and different stuff.

The pre-built blocks are placed here carefully to help us to perform our analysis without any intervention. We can see we have the simulation input glyph, this one in the corner, where we are importing all the results from the static analysis and the harmonic.

I can activate the display and I can see now my final element results, for example, from here, by right-clicking and properties, I can select the file where I want to plot the results from. For example, I have from the harmonic and from the static.

Let's say we can go to the FADisplay and select one case. We can see we have both. We have vibrations here and we should have statics from the other. Vibrations, displacement, this one for example. This is displacement from the static and this is from harmonic, all of this.

We have several results because we solve for several frequencies in our harmonic analysis and that's how we can see all those results files available. Let's check for example stress and select and apply. Ok, now we can see some of the results we are importing from the Ansys files.

This is the same we expected to see. We can reduce this glyph because here we are not doing any fatigue evaluation. We see several blocks or glyphs here where we need to do some kind of configuration.

In this case, we are concerned about the connection between the simulation input and our swept sine analysis. This glyph is the most important here because this is the solver where we are going to execute the S-N curve or a life calculation for this fatigue analysis.

We can also see, let's move a little bit these two guys, we can see we have two input paths in the swept sine analysis which are these two green input paths here I am trying to highlight.

and we have from one side we have the FRF input which means we are connecting the harmonic analysis results to this input path. In the second one we have the offset load case input. This one will allow us to introduce our static structural analysis as an offset for the harmonic analysis.

That means that will act as a mean stress where that will be the base value where all the harmonic will oscillate during the fatigue evaluation you know.

And we also have, this is important because if we want to create this in an empty space working in nCode, we need to connect both in that way to be able to combine these two different analysis types here.

We also have our vibration generator which is only a multiplier for the harmonic analysis results. That means this is a table frequency dependent and we have this factor that we are going to apply to the load level we are introducing from the finite element results.

For the same purposes, I can include or modify any of those options I have here. I can include some kind of mean stress correction, for example, by default we have this interpolate option, but we can also use, for example, Goodman, Gerber, and so on. Let's choose Goodman for this case.

And we have the engine method, which is multi-ratio curve. That means our material should have fatigue curves, S-N curves, defined based on the ratio. And this is important because we need to be sure our material data is corresponding properly with our nCode analysis.

Doing so, we will be successful during this analysis.

I am going to scroll down a little bit more and because we are trying to solve for one frequency, imagining maybe this load can be generated in our component by, I don't know, an oscillator or just the vibration from a motor or so on, we can say, okay, we are only interested in one frequency.

Doing so, we can modify this sine sweep property, which is the vibration loading method. I'm going to change it by, instead of sine sweep, I'm going to use sine dwell, which is the property for this purpose.

And then I can define my duration seconds, let's say 10 seconds, and the frequency I want to solve for. This is just a frequency 20 Hz. Okay, I already have my setup here. I'm going to click apply and then okay. Good. The last step here will be right-click again and edit the load mapping.

I have now this message that indicates me it's gonna run some part of the workflow and I'm gonna say yes. And I have my load mapping here. This is important because here we need to specify how we are going to include all the loads. We have four tabs here. We have model F ref static and temperature.

If we go to the frequency we can see the frequency and the result file is already loaded in the load case. We don't have any factor applicable here because I already created it by my vibration generator. That's why we don't have the possibility to modify it here.

But if I go to the static tab we can see the file which is available but it is not loaded into my case. I need to hit this button to append this file. Highlighting here. And then I can use the scale factor to modify the value if I want to do so. Then I can hit the OK button.

And at this point we are able to run our analysis. We just need to hit the play button and wait for the analysis to solve. Excellent! Now our analysis is complete and we can see we have for example we have a big numerical list that we can use to evaluate each node in our analysis.

For example, we can see the most important values, could be for example the damage, here if I hit this I will sort the list, we can see the damage per node, we can see the mean stress, the largest stress, the material, and the life calculated for each one of them.

If we want to look into graphical results we can amplify this glyph which is the same results but in this case is graphical. We can see, for example, let's say properties. I am going to change my visualization to instead of using the damage results I want to see, for example, the mean stress.

If everything is well considered in my analysis, my mean stress will be close to the actual stress developed by the load I apply in my static analysis, that means something close to 10 MPa. We can see the yellow color band is in this range, which is very close to 10 in this case.

This is what we expected. That means it is considering properly our analysis. We can move, for example, again to properties, and we can see the amplitude, the stress amplitude. Selecting this option and hitting OK.

And now we can see we have in this region, this is around 25 MPa, which is pretty close with the analysis we previously defined in the harmonic part of the analysis. And the last we can see life and damage if we want, just to consider the valuation of our part. Let's say life and okay.

Okay, this is what we have, in this case, those are cycles we need to multiply by the frequency to calculate seconds, but we can evaluate for each part the life depending on the frequency we applied into our simulation.

This is all for this video, I expect that will be useful for you and allow you to combine any static result with harmonic analysis in fatigue evaluation. Please contact us at https://ozeninc.com/contact for more information.