Step-by-Step Tutorial: Homework of Session 1


#1

NOTE: This is an update to the first version of the tutorial since the platform was updated on 01/08/2016

Recording

Homework submission

Submitting all three homework assignments will qualify you for a free Professional Training (value of 500€), a certificate of participation and will give you a chance to win a fully-working prototype of a 3D printer with your design modifications.

Homework 1 - Deadline 29.02 12:00pm

Please use this form to submit your homework

Exercise

Our aim is to investigate the heat transfer through the assembly to get insights about the temperature distribution within the extruder. This will help us on the one hand to understand the melting process itself and in addition also help us to verify the position of the temperature sensor for the closed-loop control system of the extruder.

We will therefore investigate the temperature distribution for four different resistor temperatures (400 K, 420 K, 440 K, 460 K).

Please submit your homework using the form we provide. Please keep also in mind that your homework project needs to be public!

Step by Step Instructions

Meshing

First of all you have to import the geometry into your SimScale workspace.

  • To make this project public, click on the project name in the top left and edit the project properties and change the visibility to public.


  • Click on the New Mesh item in the project tree. This will open an additional column in the middle.

  • 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
  • Save the settings by clicking on Save button and then start the meshing operation by clicking on Start button.

The mesh computation takes around 10 min to complete and you will see a finished status in lower left corner.

Simulation Setup

  • Switch to the Simulation Designer by clicking the related button in the main ribbon bar and then click on New button to create a new simulation set up.

  • Give the simulation set up a suitable name - Simulation 1(optional)

  • Since we are interested in studying the temperature distribution of extruder, select Heat transfer under Thermostructural analysis.

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 Extruder_Mesh in the middle column. Don’t forget to save your selection.

Contacts

Since we are simulating an assembly of two parts, it is necessary to define the interactions within the assembly and with its environment. We will therefore define Contacts which covers the physical interaction between parts. Without the contacts, the solver won’t have any information about how different parts are connected to each other.


Important Note: During the webinar we showed a slightly different workflow for this: Instead of creating Topological Entity Sets first, we will will directly assign the faces to the contacts

  • Click on the Contacts sub-item in the project tree. This will open a new middle column windows where you can manage existing and create new contacts.

  • Next, click on the New button to create a new contact definition.

  • For every contact definition given below, use Add Selection from viewer button in the bottom of Master/Slave Entity section after selecting the corresponding faces to assign the faces graphically and click on Save button to save the settings.

Contact #1 - Heat block, Nut and Nozzle
This contact is necessary to connect the heat block and the nut with the nozzle.

  • Specify the following parameters:
  • Name: Contact 1
  • Type: Bonded Contact
  • Master entity: faceGroupOnGeoFaces_50 (volumeOnGeoVolumes2), faceGroupOnGeoFaces_61 (volumeOnGeoVolumes3)
  • Slave entity: faceGroupOnGeoFaces_39 (volumeOnGeoVolumes1)

Contact #2 - Heat sink and Nozzle
This contact is necessary to connect the heat sink with the nozzle.

  • Specify the following parameters:
  • Name: Contact 2
  • Type: Bonded Contact
  • Master entity: faceGroupOnGeoFaces_0(volumeOnGeoVolumes0), faceGroupOnGeoFaces_1 (volumeOnGeoVolumes0)
  • Slave entity: faceGroupOnGeoFaces_37 (volumeOnGeoVolumes1), faceGroupOnGeoFaces_41(volumeOnGeoVolumes1)


Contact #3 - Heat block and Nozzle
This contact is necessary to connect the heatblock with the nozzle.

  • Specify the following parameters:
  • Name: Contact 3
  • Type: Bonded Contact
  • Master entity: faceGroupOnGeoFaces_46(volumeOnGeoVolumes2)
  • Slave entity: faceGroupOnGeoFaces_35 (volumeOnGeoVolumes1)


Contact #4 - Heat block and Nut
This contact is necessary to connect the heat block with the nut

  • Specify the following parameters:
  • Name: Contact 4
  • Type: Bonded Contact
  • Master entity: faceGroupOnGeoFaces_45(volumeOnGeoVolumes2)
  • Slave entity: faceGroupOnGeoFaces_59 (volumeOnGeoVolumes3)


Materials

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 New button

This will open a middle column windows where you can specify material models and apply them on different volumes of your mesh.

  • The standard values for Density and Conductivity are for steel. Since the whole assembly is made of steel, you can simply assign the material to all volumes of your mesh.

Initial Conditions

Next we take a look at the initial conditions.

  • Click on the Initial Conditions sub-item.

The Initial Conditions define the initial values for Temperature. To understand this you have to keep in mind how engineering simulation actually works: Since the mathematical equations fluids can only be solved numerically, the solver needs an initial solution to iterate. In some special cases it can be necessary to adapt this in order to make the simulation more stable.

  • Since the default value of 293.15 K is fine for us (approx. 20°C) we don’t have to touch it!

Boundary Conditions

Now you can start to specify the physical behaviour of the extruder and its interaction with the environment by defining the Boundary Conditions for all faces of the mesh.

  • Click on the Boundary Condition item in the project tree which will open a new column in the middle of the windows. Here you can see an overview of all boundary conditions which are applied to your mesh.

First we will specify the temperature boundary condition to describe the heat of the resistor which is transferred through the heat block into our assembly

  • Click on Temperature Loads under Boundary Conditons in the project tree and then click on New button.

This will add a sub-item to the project list and open again a new window where you can define the boundary condition. Here you can define a name for the boundary condition, choose the type and assign it to faces by using the list below.

  • Specify the following parameters:
  • Name: Resistor
  • Type: Fixed value
  • T[k]: 400
  • Please map this boundary condition to the bigger hole of the heat block: faceGroupOnGeoFaces_44 (volumeOnGeoVolumes_2). To assign the face graphically, click on Add selection from viewer after selecting the corresponding face.

Next, we will add Heat flux Loads to describe the heat exchange with the environment through the outer surfaces.

  • To do that, click on Heat Flux Loads option in the project tree and click on New button.

  • Specify the following parameters:
  • Name: Convection
  • Type: Convective heat flux
  • Reference temperature [k]: 293.15
  • h[W/(m²K)]: 5
  • Map this boundary condition to all surrounding surfaces of the assembly (except contacts and the surface where you applied the resistor boundary condition). Use Add selection from viewer button to assign the faces graphically as in the previous boundary condition.



  • Finally Save the settings after assigning all the faces to the bondary condition.

Since it is not necessary to edit the Numerical Settings we can just skip this section.

Simulation Control

Before we can start our simulation, we have to define the settings of our simulation under Simulation Control.

  • Specify the following parameters:
  • Pseudo timestepping: Single step
  • Number of computing cores: 4
  • Maximum runtime: 3600

Simulation run

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

  • You can now start the simulation run by selecting it from the project tree and then click on the Start button.

The run will take approximately 2 minutes to complete. After the run is finished, you will see Finished status as shown in figure below.


For simulating the other temperature load cases, change the related boundary condition and create a new simulation run!

Post-processing

  • Once your simulation is finished, click on the Post-Processor button in the main ribbon bar and then on Solution field under Run 1 to view the result.

To take a look inside the assembly, we will apply a Clip filter.

  • Click on Add Filter button and then select Clip from the list.

  • You can control the clip plane by specifying normal and origin:

  • Select temperature [point data] in field [1] to view the temperature distribution.
  • Select toggle color bar to view the temperature scale [2].
  • You can hide the clip plane by unchecking the Show Plane option [3].


#2

#3

#4

#5

#6

Hello,
I’m trying to submit the homework by using the linked form, but after entering my mail adress and the link I generated via the share project button the form just leads to a 404 error page. Did anyone already submit the homework successfully?


#7

Hi @PascalBeike, we’ve edited the submission form, could you try again and let me know?


#8

Tried it again: submitting the form leads to the front page of the 3D Printer Workshop now. Apparently the form actually worked before (I received a mail which stated that the homework was received), there was just no confirmation in the browser window.


#9

Ok thanks for making us aware of that - also fixed!


#10

Should we exclude both contact entities (master and slave) when applying the heat-flux BC?


#11

Hey,

Yes please exclude all contact entities (master and slave) since there (should) be no convective heat transfer between the surfaces.

Cheers,

Milad


#12

Hello,

some surfaces of the heat block and the nozzle are partly in contact with other parts and partly with the environment (face 45, 46, 39). Also some surfaces are covered by other parts. Does the program automatically distinguish which part of the surface is contact with air?

Cheers,
Thorsten


#13

Hi, I am playing around with the HW01

I have two questions:

I would like to apply heat source as concentrated heat flux, say 40 [W], how is this possible on a surface (currently I can only choose nodes /node sets) ?
I would also like to know the surface area of the insert (for heat cartridge), is there a measurment tool to find this area ?


#14

Hey @srosendal,

a concentrated heat flux is used to introduce heat as a point source. If you add it on multiple nodes it will be added on all of those nodes with the same magnitude.

I you want to introduce heat via a surface, you should use the surface heat flux boundary condition. Right now you need to add a value based on the unit surface area W/m², so you need to know the surface area of the face if you want to introduce an absolute value (W). We are working on a new setup, where you can make this optional (either use an absolute W value, if you do not know the surface area or a relative area based value, if you do not know the total amount of heat). Until then you need to check on the size of the surface area in your CAD-tool.

Best Alex


#15

Ok, thanks a lot for your response

I just wanted an option that let me apply heat [W] to all nodes of a selected surface. It sounds great you are now working on this option, in the meantime I use the [W/m^2] option.

Are you also planning on implementing a measurement tool ?


#16

Hello @Thorsten

In order to make any face to be in contact with air, you need to assign a dedicated boundary condition (for example buoyant heat flux condition).
Any face that does not have a BC prescribed is assumed to be adiabatic.

This might indeed bring trouble if a face is partially exposed to air, and partially in contact with other elements. If you have the body being cooled by all its outside surface, the best practice is to have the the contact faces separated to the contact part and the cooling part. It requires a bit more work with the CAD but the results will be more accurate.

Best,
Pawel