To preface, these are notes I took when learning how to do the sim set up for our current Billet trailing arm design (see pictures below), courtesy of Advait Joshi’s guidance. In my opinion, I felt that this was great sim to learn in general over Ansys mechanical, engineering design principles, and that was not too easy/simple but also not overly complex---it was the right amount of difficulty.

This walkthrough explains everything from the moment you open Ansys to the final sim results and how to properly interpret them. If you have any questions, as always, feel free to reach out…Yuh.

FINAL NOTE: There are in notes in orange for areas for improving this sim; Of course, this sim is still a work in progress so this page may be updated over time → not fully finalized…

Also tried to be very thorough so might seem long but not too bad once you get the hang of it/do a couple sim iterations

Thanks,

Joshua Palacios

Part 1 - Setting Up in Ansys Workbench:

Before opening Ansys, make sure you are connected to Cisco VPN if you are not on a UT wifi (e.g. trying to sim from home)

Download the below file ‘Min Materials’ if you haven’t already--this is your engineering data file

After launching Ansys Workbench, in the new project window, drag out ‘Engineering Data’ box from the sidebar
1. right click on Engineering Data > click edit > opens a new eng data tab
2. import the Min Materials file as the engineering data
3. shift click on the first material, scroll to the bottom of the list and click on the last one – should highlight/select all materials
4. unselect the part material – for the billet trailing arm unselect Aluminum 6061-T6 with cntrl click and delete the rest of the materials
  1. the reason for this is b/c only need the one material for the sim + the file has undefine materials that if we wanted to keep would have to define their properties (time waste)
Now go back to the ‘project tab’ and drag out in ‘Geometry’ from the sidebar
1. import from Solidworks your trailing arm assembly as a Parasolid file
2. right click > edit geom in spaceclaim > wait for it to load
3. suppress everything that is not the trailing arm itself, i.e. the of rest of wheel assembly
4. The trailing arm assembly should end up looking like this after you suppress everything not needed
  1. Leave the motor + caliper mount, t-arm body, pushrod tab, and the pushrod itself
    1. hide all hardware (Rodends, bolts, etc.)
Then go back to project and drag out Static Structural
1. drag eng data and geometry into their respective boxes
  1. Your project tab should now look like the image below with the checkmarks:

Part 2 - Setup in Static Structural

Now double click on ‘model’ (the 4th row option in the static structural box (see pic above)
1. Ansys Mechanical window will now open
2. In the sidebar, click on plus box in ‘connection’
3. click on ‘contacts’
  1. Ansys automatically identifies contacts for you but we will need to fix these (explained below)
  2. This is what you window should look like right now
Contacts and Joints
1. Setting Up Contacts
2. There are 4 contact regions:
  1. 1st: flip pushrod and insert contact/target
    1. you want ‘target’ to be less deformable one
      1. usually deciding which one this is in just thinking about it intuitively
    2. in this case is is the AL insert going into the pushrod
      1. assume the the rod is AL, even though it’ll be carbon fiber (CF); doesn’t matter here
    3. ‘Contact Region 1' will now auto rename to 'bonded’
  2. 2nd: motor mount is less deformable so set that one as ‘target' (contact is pushrod tab)
    1. Ansys should already have it like this; just double check but shouldn’t need to change this one
  3. 3rd: Flip this one; set trailing arm body as target; motor mount is the contact
  4. 4th contact is fine
3. Contacts are done now
4. NOTE: 2 different type of connections exist
  1. 1st is contacts which is like frictional and bonded ones
  2. 2nd is joints → joints fix/create relationships between fixed objects
  3. ‘Connections’ in sidebar will look like this once we set joints up now
  5. NEED TO ADD 3 JOINTS FOR THE FRAME TABS AND 3 RODENDS
5. Setting Up Joints
  1. click on the face you want joint at; then go to ‘body-ground' (top bar) then click 'spherical joint’
    1. body and ground is making a relationship with that point in space at that current time
    2. body to body creates a relationship between two bodies; links motions; rather than a point in space → will use it later (4th joint)
  2. go to ‘face selects’ (top bar) and select the face one to make it easier to select faces; select the face of the pushrod rod 1st (see 2nd pic below)
  3. Example of Rod end face; Note: technically could be more accurate here since the rodend isn’t actually this entire face…something to look more into the future to make the sim more accurate
    Pushrod tab face selected
  4. Click ‘general joint’ → here we are basically defining our own stiffnesses and rotations;
  6. As shown in the above picture, next to ‘rotation’ (highlighted in blue), set as ‘Free in X’
    1. set as ‘fixed’ in all translations
    2. side note: cntrl-middle mouse button to move around easily
    3. This general joint is your rodend joint; your pushrod is fixed in the X direction but can move in the z-y plane, i.e. as the shock is compressed or decompresses
    4. your other 2 joints are the rodend joints connecting to the frame; set these as ‘spherical joints’ (see pic above) →
  7. IMPORTANT: go back to all joints and FIX the coordinate system
    1. in the future, do this while you make the joints
    2. This basically means clicking on the arrows at your joint until it matches the coord system at the bottom right of the window (just keep clicking on them)
    3. if you don’t do this; it essentially won’t make your joint ‘true’
  8. SIDENOTE: reason we don’t use hardware instead set all of these ‘boundary conditions’ is b/c hardware gives funky results in Ansys
  9. Now make the 4th joint
    1. click body to body; click round holes faces in pushrod tab
    2. then click 'no selection' (top box) -> when there is an orange box you have to fix it
    3. clicking ‘no selection’ applied the geometry to the selected faces (see pic below)
    5. then click the rodend face touching the pushrod which is the inside the AL insert (see pic below)
    6. inside of insert face selected
    7. double click ‘no selection’ again
      1. basically this makes it so they are locked in translation but can rotate together
    8. Now Joints are done

Part 3 - Meshing and Running the Sim

Change units from metric to mm kg (bottom right)
Now click on ‘Mesh’ in the side bar
1. do a 3mm mesh; click on ‘element size' and put in 3 for 3mm mesh (pic below)
NOTE: Always make sure when simming that all meshes are at least 3 elements thick (rule of thumb)
Now right click ‘mesh’ and click ‘generate mesh’
3mm Mesh generated
Now click ‘Static Structural' (still in this Ansys mechanical window)
then click loads and remote force in top bar
1. static structural is where you add all remote loads and supports
2. sidenote: bolt pretension IRL is present; that's a type of support but something to figure out in the future for improving this sim…
REMOTE FORCE 1:
cntrl click all 6 motor bolt holes since that's where the force is coming from; then will scope from there later
then click 'apply' for applying the selection geometry (see pic above)
Now put in coord pts (got these from CAD) of the contact patch
1. this is where we are saying our forces are being applied → 3g bump; 1g steer
2. coords: x is 0, y is -50mm, z is -2250mm
3. Coords and Forces from Contact Patch
4. then after that click on ‘vector’; change to components and then do x = 1000N; y = 3000N; your forces from the contact patch (see pic above)
5. NOTE: this is just a rough estimate of our forces; we got these values from our expected weight of the car; look at dyn sheet 24
  1. we are just using the weight on the back of the wheel which is currently expected to be 35-40% weight in the rear based on our goal suspension kinematics (note: make sure this is set in stone with suspension people lol)
REMOTE FORCE 2:
1. control click two bolt holes for brake force (see pic) → brake force will be 2nd remote force
2. brake force application location
3. NOTE: caliper mount location will change since we are currently switching from using 2 to 1 calipers in our rear wheel (CAD in progress of being updated) → hence why we are only selecting 2 bolt holes instead of the four holes you can see in this specific trailing arm iteration
4. click on ‘loads’ then ‘remote force’ in top bar again
5. then click define by: vector; change to components → we will always define by components
  1. Pic showing Coords
6. See above pic for coords: x is 35mm, y is 303.83mm, z is -2388.1mm
7. Again: note: parking brake (our 2nd caliper) caliper does not matter here
  - Reiterating here: this ofc will change location when we switch cad to the 1 caliper; but same concept
8. NOTE: Saying we have 4000N of braking force (900N and 200N as y and z components → gives 4000N with Pythagorean theorem); should do Pythagorean theorem for more accurate number → place for improving accuracy of sim
  1. reason for this is b/c want force to be tangent to the brake rotor, estimating for now/eyeballing
9. assume force direction is upwards, prob worst case scenario; should check both just in case
  1. NOTE: braking is a force; test both directions just in case; it’s a frictional force from the calipers; not a moment
  2. for the hand calc we did previously; we did accel force on the whole arm (inaccurate and will be fixed next time we do the hand calc)
10. Brake force w/ direction and components shown

Click on ‘Solution’ now

right click then insert > stress > equivalent (von mises)
right click then insert > stress tool > max equivalent stress
right click then insert > probe > joint probe (insert 4 of these)
Inserting Things Under Solution
then go to boundary condition (orange box) and drop down menu and select the joint
1. repeat this for 3 joints; will have 3 joint probes at the end
  1. don't want the joint between the pushrod tab and rod; that pt just doesn't give any useful info
Defining Geometry Material
1. ? mark on geometry b/c need to define material first before solving
  1. shift click 1st geom then click 2nd one
  3. orange box in ‘assignment’ > go to drop down menu and select Al
    Assigning AL 6061-T6 as material
2. Geometry is now all green check marks
Now you can click Solve! (top left lightning arrow)
1. click allow on all popups to go thru firewall → those error pop ups bottom right don't mean anything (don't worry about them basically)now when solved:

Part 4 - Interpreting Sim Results (The End)

Now once the Sim Solves
1. can click on ‘solutions’: equivalent stress or stress tool>safety factor
2. can see where its failing
FOS is most straight forward
1. TIP: if you get stress singularities; then you can refine mesh size OR preferably try first changing contacts (like flipping body or target)
2. refining mesh might just make the stress singularity worse
FOS sim result
Now for ‘equivalent stress'
1. NOTES: we are using Von Mises → comparing to tensile yield strength → that's what is generally used
  1. since its a metal; compressive and tensile are pretty much the same value
  2. von mises also accounts for shear
    1. can change to tresca if you choose specifically shear strength but over approximates your shear failure; shear yield strength is calc by doing tensile/root 3 → not considering tensile and comp failure → just comparing to your shear strength
    2. von mises approx is the root 3
    3. von mises is a way of combining forces so you have a combined failure
2. you can probe in the equivalent stress sim result to see max, min, and all stresses at different locations
3. if you see a stress concentration with a big jump; likely a stress singularity; so either make mesh finer or add fillet in CAD (example below):
  1. making mesh finer will likely increase stress singularity b/c smaller area (see 3rd pic below)
4. Stress Singularity
  FOS graph again

Now with a 2mm mesh → finer mesh but stress singularity value went up

LAST THING: DON'T Forget to save everything now

everything is saved through workbench
refresh project for all checkmarks
file → save as → save entire sim

Congrats, you finished a trailing arm sim!

Now what? Can do more sim iterations and optimize CAD (remove stress singularities, add or remove material where failing or passing respectively)
Sim set up for tubular design will be a bit different, similar concepts… but work in progress right now