Step-by-step guide

Edit March 6, 2019: Used SolidWorks 2018 for this guide.

Definitions

Let's start with a few definitions.

A mold is a 3D negative part of an object with the goal of capturing all geometric features of the original part.

Moldmaking is the process of creating the 3D negative space to allow for creating reproductions that are identical to the original part.

A cast is the reproduction of the original part. Casts can be made from different materials depending on the requirements.

Casting is the process of reproducing the original part. The process consists of filling the mold cavity (or cavities) with materials that hardens (typically polymers - more on materials in Mold Materials, Mold Processes) and then removed from the mold once cured. Depending on the mold materials, casting can occur multiple times within the same mold.

The process of curing is the hardening of polymer materials.

Casting Production Cycle:

Preparation of Material
Filling the Cavity
Curing Processing time
Cooling/solidifying of the cast
Ejection from mold

(For the purposes of Midnight Sun, we use molds (styrofoam, MDF, or others) to create the aerobody using materials such as carbon fiber.)

Design Considerations

In general, considerations must be made for mold design in any application, especially in mass manufacturing.

Repeatability: The mold should be able to be used multiple times, each producing a replica of the original part.

Efficiency: uses the available technology to minimize waste, optimize production, and reduce time.

Quality: These are the standards set by an industry or policies. In any case, quality is the ratio of value to cost. Does the product create enough value to the user for its cost?

Tolerances: This is the allowable margin of error or variations that is acceptable for reproductions of the original part. This would impact assemblies of objects, enclosures, open parts, and others.

Regardless of what type of mold and process is used, the reproduced part must be able to be removed from the mold. The more complicated the design is, the more difficult it gets to remove, thus designs must account for these properties.

Draft angles, the angle of taper away from the perpendicular (degrees), that are added to SolidWorks models to aid the removal of the object. More drafts are added depending on the complexity and textures in the design.

Fillets are rounded edges included in designs to facilitate the smooth flow of the cast material into the mold. Otherwise, issues such as air bubbles and will add stress to the part.

Vents are built in (depending on the casting process used) to allow for air to be better displaced by the casting material.

Creating Molds in SolidWorks

(Finally here, eh?)

Let's start with some simple models in SolidWorks to create molds out of. The method we are using is to create the negative space around the part. This would include intersecting the part with a "block" and removing the intersected space.

Simple Mold (with a symmetrical shape) - TO BE EDITED

You can use any simple shape (sphere, rectangular prism, block, etc.) but for the purposes of this section, we will be using a sphere (sphere.SLDPRT). (Please see SolidWorks Basics for instructions on how to create these shapes.)

To create a mold from the intersection between two (or more) shapes, you will be using the shape, in this tutorial, a sphere, and create a separate a New Part that is a solid block. Choose the Front Plane and use the option to draw a rectangle from the center of the plane. In this case, it does not matter what plane is used, as a sphere is symmetrical in all axis. Next, add dimensions. A key tip for this is to make the block larger than the sphere. If the block is smaller than the sphere, you can still adjust its dimensions after the mold is complete. You can use the diameter of the sphere as a reference of the block's size.

Once you have these two parts, create a new Assembly in SolidWorks. You will be prompted to insert a part - insert the sphere first and place it (left-click once you select the location) onto the document. Next, go to Insert Component and select the block.

Place the block near the sphere and overlap it if possible. It does not need to be perfect as you can use the different view to drag and drop the block to the desired location. For example, you can view a perspective orthographic to the front plane and move the block along that axis. Repeat for the other views to move the block on those axis and aim to intersect approximately half of the sphere will the block. It is good practice to center the sphere into the block if the block needs to be adjusted later. You may result in the following views:

Next, select the block. Go to Assembly > Edit Component:

Then Insert > Features > Cavity.

A Property Manager will appear and prompt you to select the part that you will be basing the cavity out of. The part you select will also be highlighted in blue (or other colours depending on the SolidWorks version). Note, you may need to move the perspective of the assembly in order to select the sphere.

Click the green checkmark to complete the cavity. You can also exit the Edit Component view.

To view the cavity that you created, right click the sphere part and Hide Component. This will show the block without the sphere.

Make sure that the two parts remain in their original position when the cavity is created. This will allow you to save and rebuild the parts so that the original file for the block will reflect these changes. When saving, remember to Rebuild when prompted.

Now, when you open the block's file, there will be the indentation, or space, deleted with the Cavity function. If the mold's size was not large enough to accommodate the part, you can edit the size of the mold in its respective file by changing the dimensions of the rectangle or the dimensions of the extruded boss/bass.

Congratulations! You have created your first mold!

See the following tutorial for building molds of complex, non-regular shapes.

Complex Mold (with a more sophisticated part)

For the complex mold, we will be using an aerobody as the example, as this will aid the transition of building molds for the end goal. The process is very similar to creating a Simple Mold, however, the challenging part will involve the planning and creation of separation markings, which will determine how the molds are created and have easily identifiable points to how it is connected/mounted to the rest of the car.

(Part updated on March 8, 2019,) the 3D model that is used in this example is: AerobodyAestheticModel_REV2B.SLDPRT, the current version of the MSXIV aerobody. Since this part is created already, you will only need to create the base for the mold, i.e. a rectangular block. It is recommended that the dimensions of the box is not too far fetched from the width and length of the portion of the aerobody that the mold will be made from. While this makes it more convenient for the part to be centered into the block without needing to make major changes to the block's dimension, always aim for a block with larger dimensions than smaller.

To start, create a New Part in SolidWorks. Choose the Front Plane and use the option to draw a rectangle from the center of the plane. Note, in this case, we use Front Plane because the part we want to mold, the bumper, is in that plane. For the side panels of the car, you would use the Right/Left Planes, and for the top and the bottom of the car, you would use the Top Plane. For other areas, you would need to create your own plane to be optimal for the aerobody. In this example, the dimensions were 2000 mm x 1500 mm with an Extruded Boss/Base of 1000 mm.

The part is now ready to be used in an assembly with the model. In a new Assembly document, place the aerobody onto the document first. Next, go to Insert Components and select the block you had created previously. Place this in a location that is close to the part of the aerobody that is to be molded. In this case, place the block close or overlapping with the bumper. Move the block around, changing the view plane as required so that the bumper is approximately centered into one of the faces with the largest surface areas. Make sure the car does not go through the block, i.e. you cannot see it from the other side. In terms of depth of the intersection of the block, for now, allow the overlap to be just enough for the front of the bumper. See light blue outline of the part in the second image:

Making sure the two parts, the block and the aerobody, are connected, select the block and go to Assembly > Edit Component. You will notice that the aerobody part is now an outline rather than a solid body.

Go to Insert > Features > Cavity. A property manager will appear and asks you to select a part that will make the cavity. Select the aerobody.

Keep the Scale Parameters as 0.00% for now. Note, this function can be used to create draft angles. Click the green checkmark when done.

By default, you will still be in the Edit Component view. You will see that the aerobody is still outlined, but there is now a cavity within the block. When exiting the view, both parts will be solid. Moving the block away from the aerobody part, you will see the details of the aerobody in the cavity.

NOTE: You cannot save and keep the cavity if the two parts are not connected. In this step, undo until the parts are connected right after the cavity is created.

When saving, be sure to rebuild the parts. This will allow the changes to be reflected to the block in its original part file.

You have created your first mold of the aerobody!

Creating Molds through SolidWorks Mold Tools

Draft + Draft Analysis
Parting Lines
Parting Surface
Shut-off surfaces
Tooling Split