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How to Create a Three (or More!) Piece Mold in SOLIDWORKS

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For most mold designs, we split the mold tooling into two halves: a core side and a cavity side. However, splitting the tooling into three or more pieces works better for some designs.

While this functionality is unavailable in the normal tooling split command in SOLIDWORKS (you can only use one continuous parting surface), we can still achieve it with a few extra steps. Because this is a more advanced mold-making technique, this blog will assume you are already familiar with the standard mold design process in SOLIDWORKS.

Method 1: Continuing with Mold Design Tools

This method uses the typical mold design tools to create a tooling split of the core and cavity. Then, you can further split the core or the cavity (or both) to create extra tooling. You can accomplish this most easily by creating a surface and then using the split command.

SOLIDWORKS model of a mold
Figure 1: The mold halves are shown in green and blue, the red geometry is the runner for this part. Due to the limitations of the Tooling Split command, the red runner cannot penetrate the mold tooling and would need to be opened up manually afterwards.

First, offset a surface from the bottom of the molded part and extend it until the surface is larger than the existing tooling. This will separate the runner geometry into a new tooling block.

SOLIDWORKS mold model with surface offset from the bottom face
Figure 2: A surface is offset from the bottom face of the molded part.
SOLIDWORKS mold model with surface extended
Figure 3: Then the surface is extended to be bigger than the mold tooling.

Then, use the split command to cut the mold body into two separate bodies with the newly created surface.

Use split command in SOLIDWORKS to create two bodies
Figure 4: The split command will create two bodies from the bottom half of the mold.
SOLIDWORKS mold model with three bodies
Figure 6: The three mold bodies shown in green, blue, and orange.

This results in three separate tooling bodies that you can insert into the larger mold assembly to manufacture the part and its attached runner.

Method 2: Using Surfacing Techniques

Sometimes, it’s simpler to forego the normal tooling split command and use manual surfacing techniques. This can be useful for more complex parts where the standard mold commands may not work well or at all. It can also be helpful if you are already familiar with the surfacing workflow and don’t want to use the mold commands in SOLIDWORKS.

To get started, make a ruled surface around the top edge of the box, perpendicular to the direction of the pull.

SOLIDWORKS mold box with ruled surface
Figure 7: A ruled surface is made around the top edge of the box

Next, construct a secondary parting surface. This is simply offset from the bottom of the molded part and then extended in all directions. In other words, you can make it in the same way as the first method.

Create a second parting surface in SOLIDWORKS
Figure 8: A second parting surface is made, using the offset and extend surface commands.

Using an extrude, make a solid body around the molded part. In this case, the mold tooling will be rectangular but can be any shape. The merge result checkbox is cleared to leave the extrude as a separate solid body.

Keep the mold tooling as a separate body in the 3D CAD model
Figure 9: The merge result checkbox is cleared when extruding, in order to keep the mold tooling as a separate body.

Next, hollow out the mold tooling body with the Combine command using the subtract option.

Subtracting a body to create a cavity in the mold model in SOLIDWORKS

Figure 10: The plastic part is subtracted from the mold block to create a cavity. Note that this will consume the part body.

Then, apply the Split command to split the tooling into three separate bodies, using both surfaces created earlier (the ruled surface and offset surface).

Three body mold CAD model after split
Figure 11: Three bodies are created as a result of the split.

Using two surfaces in SOLIDWORKS to split the mold tooling body

Figure 12: The two surfaces are used to split the mold tooling body.

While the two surfaces were created here using a Ruled Surface and Offset Surface command, you could use any surfacing techniques. In addition, you could use any number of surfaces to generate more independent mold bodies.

Final 3 piece mold in SOLIDWORKS
Figure 13: The final result. Note how the runner opening exits the bottom of the tooling in this example.

Choosing the Right Technique for Mold Splitting

Either one of these techniques would allow the creation of a mold with three or more bodies. They both differ from the Core command in the Mold Tools because they are based on surfaces instead of sketches. Therefore, the Core command is typically better for removing smaller sections of the mold, while these techniques are better for splitting the mold entirely into large equal sections.

One notable difference between the first and second methods shown here is that the first uses the conventional Tooling Split command. This means the runner cannot pass outside the mold, and you’d need to create a hole afterwards. The second uses purely surfacing commands so the runner can immediately penetrate the outside of the tooling.

The first technique can be helpful for users already familiar with the mold-making commands in SOLIDWORKS or for models originally designed with two mold halves that need to later be divided further into more individual tooling blocks.

The second technique may be better for more complex ground-up designs, as the surfacing commands generally offer a finer level of control.

Have questions? Contact us today or check out some of our other mold making tutorial blogs, including topics such as the Parting Surface command, Parting Line command and the Shut-Off Surface command.

Picture of Kenny Truong

Kenny Truong

Kenny Truong is an Applications Engineer based out of our Brooklyn Park, MN office. He comes from a background of engineering at a local startup and student teaching at the University of Minnesota. He specializes in SOLIDWORKS 3D modeling.
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