SimScale CAE Forum

Step-by-Step Tutorial: Homework of Session 2


#1

> NOTE: This tutorial was updated on 08/2016 to match the updated version of the platform

Exercise

Our aim is to investigate the mechanical behaviour of the frame of the 3D printer. We will therefore run two different simulations. First of all, we have to identify the critical eigenfrequencies of the printer frame. Later on, this information will be used as an input to analyze the physical response of our system.

Step-by-Step Instructions

Meshing

First of all you have to import the geometry into your SimScale workspace. For this, you only have to click on this link. Please note that this can take several minutes.

Now, click on the Meshes item in the project tree. This will open an additional column in the middle.

Next click the Create new mesh button to generate a new mesh.

First you have to define which geometry you want to mesh by choosing the related geometry from the Base drop-down menu. Choose ‘Chassis_Arm_Simplified’ and click the Save button below.

Next, click on the Add mesh operation button to create a mesh based on the geometry you selected before. This will open a new middle menu where you can specify the mesh operation you want to use to create the mesh.

Select Tetrahedral Automatic from the list and choose the following settings

  • Specify the desired mesh order: First order
  • Fineness: 3 - Moderate
  • Number of computing cores: 4

Now, click on save to save the meshing settings.

Once done, click save and start the meshing process by clicking on the start button at top. The meshing process will take less than 10 minutes to finish.

You will be notified once the mesh is computed

Simulation Setup I

Please switch to the Simulation Designer by clicking the related button in the main ribbon bar

Click on the New simulation button to create a simulation run. This will open an additional column in the middle. Here you can select which kind of simulation you want to run.

In our case we will run a Frequency analyis to recive critical frequencies for the harmonic analyisis.

Next you have to specify which mesh you want to use for your simulation. Click on the Domain item in the project tree and select Mesh 1 from the menu which disappears in the middle column. Don’t forget to save your selection.

Since we are simulating an assembly of parts it is necessary to define the interactions withing the assembly and with its environment. We will therefore define this so called Contacts, which are also covering the physical interaction between parts. This topic was also covered very detailed during the last webinar. You can find the section about contacts here

Without the contacts, the solver does not knows which parts are connected to each other. To define the full interactions between the six different solids we need at least nine contacs.

Please click on the Contacts sub-item in them project tree. This will open a new middle column windows where you can manage exisiting and create new contacts.

Next, click on the Add contact button

Contact #1 - Connector (solid_3) and Rod (solid_1)
This contact is necessary to connect the Connector (solid_3) and Rod (solid_1)

  • Name: Contact_3_0
  • Type: Bonded Contact
  • Master entity: faceGroupOnGeoFaces_393 (volumeOnGeoVolumes3), faceGroupOnGeoFaces_386 (volumeOnGeoVolumes3)
  • Slave entity: faceGroupOnGeoFaces_73 (volumeOnGeoVolumes1), faceGroupOnGeoFaces_212 (volumeOnGeoVolumes1)

Contact #2 - Connector (solid_3) and Rod (solid_0)
This contact is necessary to connect the Connector (solid_3) and Rod (solid_1)

  • Name: Contact_3_1
  • Type: Bonded Contact
  • Master entity: faceGroupOnGeoFaces_392 (volumeOnGeoVolumes3), faceGroupOnGeoFaces_387 (volumeOnGeoVolumes3)
  • Slave entity: faceGroupOnGeoFaces_4 (volumeOnGeoVolumes0), faceGroupOnGeoFaces_58(volumeOnGeoVolumes0)

Contact #3 - Connector (solid_3) and both Rods (solid_0 and solid_1)
This contact is necessary to connect the Connector (solid_3) and Rod (solid_1)

  • Name: Contact_3_2
  • Type: Bonded Contact
  • Master entity: faceGroupOnGeoFaces_405 (volumeOnGeoVolumes3), faceGroupOnGeoFaces_406 (volumeOnGeoVolumes3), faceGroupOnGeoFaces_407 (volumeOnGeoVolumes3), faceGroupOnGeoFaces_408 (volumeOnGeoVolumes3)
  • Slave entity: faceGroupOnGeoFaces_96 (volumeOnGeoVolumes1), faceGroupOnGeoFaces_99(volumeOnGeoVolumes1), faceGroupOnGeoFaces_24 (volumeOnGeoVolumes0), faceGroupOnGeoFaces_27 (volumeOnGeoVolumes0)

Please find below and overview for the missing contacts and create them:

Next we have to define the physical Model we want to use for this simulation. Click therefore on the Model item in the project tree which will open a middle column windows. Here you can define the gravitation.

  • Magnitude: 9.81
  • x value: 0
  • y value: 0
  • z value: -1

Now we define and assign material properties to the different parts. Click on the** Material item** in the project tree. This will open a middle column menu where you can edit and create materials and assign them to volumes. Click on the Add material button.

Now you can define your new material based on your own material proporties or access our Material Library which includes ready-to-use material models for several materials.

Next we will assign the steel material model to the screws and the engine. Add an additional material to your project tree.

Now we will access our material library instead of creating the material model manually. Click on the Import from material library which will open a widget.

Please select steel from the list on the left side and save your selection by clicking the related button.

Now assign the material to the rods (volumeOnGeoVolumes_0, volumeOnGeoVolumes_1, volumeOnGeoVolumes_2).

Please add a new material with following settings. Instead of using the library we have to define the material manually:

  • Name: ABS Thermoplastic
  • Young’s Modul: 1800000000
  • Poisson’s ratio: 0.35
  • Densiy: 1040

And assign it to the connectors (volumeOnGeoVolumes_3, volumeOnGeoVolumes_4, volumeOnGeoVolumes_5)

Next we can start to define the boundary conditions. Click on the Boundary Conditions item in the project tree.

There are two kinds of boundary conditions for structural simulations.

Constraint conditions are used to limit the degrees of freedom of the model. Load conditions are applying an external load to the model

Due the fact that this is only a frequency analysis we only need to define two contraint boundary conditions (external loads are not important at this stage).

Floor

This boundary condition is necessary since the printer is standing on a table and can not move up or down

  • Name: Symmetry XY-planeType:
  • Fixed Value
  • x displacement: unconstrained
  • y displacement: unconstrained
  • z displacement: prescribed with a value of 0

Holes
This boundary conditions is necessary to consider the fact that the frame section we are simulating is connected to other parts.

  • Name: Holes
  • Fixed Value
  • x displacement: prescribed with a value of 0
  • y displacement: prescribed with a value of 0
  • z displacement: prescribed with a value of 0

And assign it to faceGroupOnGeoFaces_450, faceGroupOnGeoFaces_449, faceGroupOnGeoFaces_448, faceGroupOnGeoFaces_447, faceGroupOnGeoFaces_418, faceGroupOnGeoFaces_417, faceGroupOnGeoFaces_416, faceGroupOnGeoFaces_415, faceGroupOnGeoFaces_391, faceGroupOnGeoFaces_390, faceGroupOnGeoFaces_389, faceGroupOnGeoFaces_388

Numerics, which is the next item in the project tree, can be skipped since the default settings are fine.

Click on the Simulation Control item in the project tree to specify how fast and accurate you want the simulation to be computed.

  • Numer of Computing cores: 4
  • Maximum runtime: 3600
  • Number of eigenfrequecies: 10
  • Lower frequency limit [Hz]: 0
  • Upper frequency limit [Hz]: 10000

To start the simulation, click on the Simulation Run item in the tree and click on the Create new run button at the bottom of the middle column menu. This will create a snapshot of your simulation settings as a new sub-item.

And start the simulation run by clicking the related button

When will be notified once the simulation run is finished.

Post Processing I

Now we will take a look at the results of our simulation. Since we are interested to find out the eigenfrequencies of the drone we will not perform a 3D post processing.

Please click on the Eigenfrequency plot sub-item in the project tree. This will open a graph which shows the first 10 eigenmodes and the related eigenfrequency.

Simulation Setup II

We will now create a harmonic analysis to investigate the physical response of our system.

Click on the New simulation button to create a simulation run. This will open an additional column in the middle. Here you can select which kind of simulation you want to run.

In our case we will run a Harmonic Analysis.

The next steps of the setup is equal to the Frequency Analysis of the previous section. Please assign the same mesh, create again nine contacts and add gravity. **Note: Regarding the contacts you have to set the position tolerance manually (0.001m), since there is no automatic position tolerance available for this analysis type.

Now we define and assign material properties to the different parts. Click on the** Material item** in the project tree. This will open a middle column menu where you can edit and create materials and assign them to volumes. Click on the Add material button.

Now you can define your new material based on your own material proporties or access our Material Library which includes ready-to-use material models for several materials.

Next we will assign the steel material model to the screws and the engine. Add an additional material to your project tree.

Now we will access our material library instead of creating the material model manually. Click on the Import from material library which will open a widget.

Please select steel from the list on the left side and save your selection by clicking the related button.

Change the damping properties:

  • Damping: Rayleigh Damping
  • αK: 0.00015
  • βM: 5.625

Now assign the material to the rods (volumeOnGeoVolumes_0, volumeOnGeoVolumes_1, volumeOnGeoVolumes_2).

Please add a new material with following settings. Instead of using the library we have to define the material manually:
ABS Thermoplastics

  • Name: ABS
  • Young’s Modul: 1800000000
  • Poisson’s ratio: 0.35
  • Damping: Rayleigh Damping
  • αK: 0.000037
  • βM: 1.5
  • Densiy: 1040

And assign it to the connectors (volumeOnGeoVolumes_3, volumeOnGeoVolumes_4, volumeOnGeoVolumes_5)

Please add now the same two constraint boundary conditions, which we used for the previous simulation.

Next add a Load boundary condition:

  • Name: Lift
  • Type: Force
  • fx: 2
  • fy: 0
  • fz: 0
  • Scaling: 1

Finally, assign the boundary condition to the faceGroupOnGeoFaces_394 (volumeOnGeoVolumes_3)

Click on the Simulation Control item in the project tree to specify the last details of your simulation.

Excitation frequencies: frequency list
Start frequency: 300
End frequency: 320
Frequency stepping: 10
Number of computing cores 8
Maximum runtime: 3600

Please choose the frequency band you want to investigate yourself (based on the results of the frequency analysis). At least you should create four different runs with different frequency bands

Finally create a new run and start it.


#3

#4

Question: Now we know the “eigenfrequence” and how the parts will be deformed. Is there any ambitions to change the design or are the calculated frequences not bad for the printer?
Thanks :wink:


#6

In the second simulation under “Model” it says “nothing to do”, so I guess adding gravity is not necessary/possible for the harmonic analysis?

And btw., it would be really handy if the contacts would not disappear when changing the analysis type! Then one could just duplicate the simulation and wouldn’t have to reassign all the contacts.

Cheers,
Thorsten


#7

Unfortunately, there is a small error:
Contact_4_1, Master entity should be: faceGroupOnGeoFaces_413 and faceGroupOnGeoFaces_420
but in the table is faceGroupOnGeoFaces_378 and faceGroupOnGeoFaces_218 for master and slave faces.


#8

Hey @Thorsten,

I totally agree regarding the contacts update on analysis type change. We have that on our roadmap, but although the desired behavior is quite clear and simple, it will take some time until it will be available. Thanks for the feedback, it helps us prioritize!

Best Alex


#9

Hey @tb2016,

thx for pointing that out! I will tell @Milad_Mafi to update the table. Obviously assigning the same entities will relate in an invalid contact condition.

Best Alex


#10

I just updated the table!