Tutorial: Creating a Part

Owned by Matt Suski
Last updated: Mar 04, 2019 by Robin Pearce

This tutorial is meant for team members who are just getting started on the mechanical team, or may be on another subteam and wanting to know more about what the mechanical team does. It outlines how to create a simple part (in this case a clevis) and some of the standard design rules that is standard on the team.

Making a Clevis


1.Understanding the Problem

Within Midnight Sun, it is important to have an understanding of what the part you are creating is for, and how it plays into the rest of the vehicle. All members need to be able to make design decisions, as there is much more benefit if the part is of your design, because then you can learn the most, and the team can create more parts faster


For the sake of this tutorial we will be recreating the front suspension clevis seen below

In designing a part it is important to know the constraints around it that will influence the material, geometry, and manufacturing process. You should ask the mechanical lead on the project if you are unclear on these requirements, because a few questions can save you a lot of time redoing CAD.

For this project the constraints given are as follows:

  • The axis of the hole that mounts the rod end is 20mm from the chassis
  • The rod end has an inner diameter (ID) of 8mm
  • the chassis tube that is closest to that axis is a 1" square tube, and the face is parallel to the axis
  • There will be substantial loading on this part

The last part is a little ambiguous right now, but a tutorial will be created later on simulating using solidworks simulation, which will cover this aspect more in depth. For now all it really says is that the part cannot be 3D printed, because those parts cannot be load bearing

2. Make sure you have the most recent version of GrabCAD


3. Create the Part


In Solidworks create a new part. This should be relatively straight forward.

4. Setting Up the Construction Geometry


From our requirements we know there is an axis that is 20mm from the flat face of the chassis. It is good practice to make those out of reference geometry, so that they can be modified easily later, should something in the rest of the suspension geometry change.

Create a reference plane that is coincident with the front plane

Now create a sketch and place a point 20mm away from the plane you just created. This can then be used to create an axis by selected the point, and the top plane. you should now have the axis and the plane similar to whats shown below

 


5. Creating the Base

When it comes to engineering design it is important to remember that every decision made should have a reason behind it. That being said don't feel like you have to get it right the first time. Create a sketch on the top plane and roughly outline what the clevis will look like. I have given an example geometry below but this is not the only possible way this part could be made. 

Rules for sketches:

  • All sketches must be fully defined. You will know this has happened when the sketch elements are highlighted in black
  • All dimensions must be in metric. If an imperial dimension is to be used write it in the metric decimal equivalent (ie 3.175mm instead of 1/8")

Suggestion for Sketches: Use relations to keep sketches clean

  • equal constraint on the top flat faces
  • equal relation on the two 15mm radii
  • tangency relation on all tangent geometry
  • vertical relation on the center of the 20mm radii to the origin of the sketch
  • Coincident relation of the center of the 20mm radii to the center of the axis created earlier

Reasons behind the sketch geometry

  • 6mm thickness is hard to say for now, and will make more sense once the simulation lesson comes out. Ask a mechanical lead if you need help with determining the thickness
  • 100mm width is to accommodate the hole for the rod end bolt, as well as the two bolts required for mounting to the chassis
  • 20 mm radii is to give enough clearance for the bolt for the rod end, however this could potentially be smaller
  • 15mm radii is to remove stress concentrations (see step x)
  • 23mm extrude is to match the chassis tube width that it will be mounted to. Material stock comes in imperial increments (nearest is 25.4mm, or 1"), however machinists like to have about 3mm to clean up the outer surface to hit specified tolerances


6. Creating the mounting holes, and the rod end holes

Now that we have our rough solid we can add the necessary holes into the part. We will start first with the hole for the rod end. Select the hole wizard tool, and set the standard to ansi metric. Similar to sketches, hole sizes are standardized to metric, only unless there is an off the shelf part (OTS part) that requires an imperial hole or thread.


Select a hole size of 10mm, and position it in the center of the axis created earlier. While the rod end hole is 8mm, because this part could potentially see a lot of motion, and it is load bearing, a bushing is will need to be added as well. Bushings help to ensure parts fit snugly together, and prevent two metal parts from wearing as a result of a lot of motion between them. A cross section of the clevis, rod end, and bushings can be seen below, as well as the part with the 10mm hole added.

Clevis (Silver) with two bushings added (Red), and the rod end (Black)


Now we need to add the holes for mounting. This is very much left up in the air as to how the clevis can be mounted to the chassis, but fasteners give a secure and reliable way to mount parts, that can be removed later. In terms of fastener size it should really be done by calculation, however the following rule of thumbs typically apply

M2.5, M3: Used for electrical boards, mounting non-load bearing parts, used for enclosures

M6: Used for mounting structural parts

M8: Used for mounting only the most loaded parts of the vehicle (typically suspension, or battery box)

For this part as it is a load bearing part, we will be using M6, and placing two holed on the face of the clevis that mounts to the chassis, similar to as shown below. Use a screw clearance for this hole, as it allow the part to be mounted even if there is a slight misalignment in the holes of the clevis, or in the chassis.


7. Adding Fillets to the Part

Fillets can be used for many purposes, and are generally good to all. In some cases fillets are necessary in making the part manufacturer, but typically they are used to remove sharp corners, which are natural stress concentrations. For the external fillets a 10mm radius was used, as it eliminated a lot of material while still leaving the original length of the part, which was important in this case for leaving enough material around the screw hole. An internal radius of 3.175mm was used, and this was because it allows for a ball nose cutter to be used in creating the radius (see below). This reducing machining time which can ultimately lower the cost for the team if they are purchasing the part

8. Finishing Touches

Now our part is pretty much done for now. before we can finish this part we need change the material to what it will be. It is important to change the material because it can be used later in the drawing, and it also gives an accurate weight of the part which is critical for vehicle analysis later. For this part 6061-T6 Aluminum has been chosen. This is one of the most popular alloys of aluminum, and is used my the team almost exclusively when it comes to aluminum parts (with the exception of 7075-T6 parts). Look as well at the T6, and see how the properties are different from that of the T4 alloy, and look online as to what this designation means if you do not know. 

After that it is time to save the part. Save parts always in the respective development folder, as it will only move to trunk once it has been set to become a production part. In the folder it needs to follow the standard midnight sun name convention. For now save parts as MSXXXXX-examplename where you replace "examplename" with a descriptive title. Later on the part will be given a proper number to replace the "XXXXX", and moved to trunk.


All you have to do now is push it to the GrabCAD, and make sure to add a comment so people can see what it is at a glance, and the part is finished for now.


Congratulations on creating a part. Future lessons to be posted will include creating sheet metal parts, how to create a drawing, adding the part to an assembly, and running a Solidworks Simulation