Tips for Designing Molded Parts in SOLIDWORKS – Part 1
When designing plastic parts which will be injection molded, you should:
- Use geometry and sizes which can be machined.
- Use in-house tooling.
- Avoid creating geometry which makes the mold unnecessarily complicated.
- Reduce the number of questions the mold maker has.
In today’s article, (part 1 of a 2-part series) we’ll take a look at one of the most common features in mold design – draft – and share some techniques to help streamline the manufacturing process.
Parts which are injection molded do not have vertical side walls. Instead, walls are tapered at a certain angle and this taper (known as “draft”) allows the physical parts to be ejected from the mold cavity.
Figure 1. Model with draft and without draft.
As we can see in the above image, the model on the right has a taper added to all of its side walls. We would say that the outside walls of this part have been created with 2 degrees of draft.
There are several things to consider which will help to avoid common mistakes and help to reduce the cost of the mold making process.
The first thing to determine is the appropriate amount of draft. The required amount of draft is not the same for every design. Generally speaking, the required amount of draft can be determined based on the material you are working with, and the length of the wall being drafted. If the wall is relatively short, you can use a smaller draft angle. If the wall is longer, you will need more draft to prevent these longer areas from getting stuck in the mold.
Figure 2. Certain areas of the model may require different amounts of draft.
Draft angle can be uniform for the entire model, or it can be different in different areas on the same model, depending on the geometry. We can see an example of this in the image above.
When first getting started with designing parts for injection molding, the best thing to do is to ask the mold maker how much draft they need for the parts. An experienced mold maker can help you by sharing resources and guides, as well as sharing what they have learned about certain types of parts or certain types of materials.
In House Tooling
As mentioned, the required draft angle is based on the material of the part and the length of the wall to be drafted. But sometimes a different (larger) draft angle will be used, based on the availability of tooling.
Figure 3. A tapered end mill that the mold maker has in house.
In this case, the mold maker has determined that the minimum amount of draft required for the main pocket is 2 degrees or they have asked us to create the 3D model with 3 degrees of draft because they have a 3 degree tapered end mill in house (as shown above).
If we had not spoken to the mold maker and instead created the part with 2 degrees of draft, extra time would have been spent going back and forth with the mold maker and making changes to the 3D model. For this reason, it is good to know what type of tooling the mold maker has access to and how this will affect the draft angles we add to the 3D model.
Drafted Geometry Will Change the Size of the Features
Our models are typically designed so that they can interact with other parts. In the case of today’s model, a round wooden dowel needs to fit through the large hole.
Figure 4. 9mm wooden dowel going into 10mm hole.
In the original, non-drafted model this works great. However, once we add the 5 degrees of draft to the 10mm hole, we end up with a problem.
Figure 5. After adding 5 degrees of draft, the top opening shrinks to 8.25mm.
In the original non-drafted model, the 10mm hole was large enough to accommodate the 9mm dowel. However, once we add the 5 degrees of draft, we end up with an 8.25mm opening at the top and the hole is too small.
Image 6. Edit the draft and specify the top face for the start of the draft.
Since we know this hole needs to maintain the 10mm opening, we can edit the draft feature in SOLIDWORKS and change the start of the draft to the opposite face. Once we edit the draft feature, the hole is both drafted at the required 5 degrees and large enough to accommodate the 9mm wooden dowel.
Sometimes the mold maker will ask for the original model, without draft. In situations like this, it is important that we communicate to the mold maker which dimensions are critical. If we leave the decision up to the mold maker, we could end up with parts which are unusable.
Draft and Fillets
When designing parts with draft in SOLIDWORKS, you will have to consider the following question:
Do I add the fillets first and then add draft? Or do I add the draft first and then add fillets? The answer to this question is: It depends! We have to think about the manufacturing process.
Earlier, we discussed the idea of cutting the 3 degree drafted pocket using a tapered end mill. When it comes to fillets, we have to think about this 3 degree taper and we may need to consider the use of another tool—a tapered ball end mill.
Figure 7. Tapered ball end mill.
A tapered end mill allows us to cut the main pocket with a 3 degree draft and will result in sharp corners at the bottom of the pocket. A tapered ball end mill will cut the main pocket with a 3 degree draft with a radius in the lower corner of the pocket. This will result in a conical surface in the larger corners of the pocket, where the tapered part of the tool is cutting the material (shown in red above). At the same time, we will be cutting a smaller constant radius around the bottom of the pocket, where the spherical part of the tool is cutting the material (shown in yellow above). Some of the fillets will be conical (or tapered) and some will have a constant radius.
Figure 8. Order of fillets and draft in the SOLIDWORKS model.
Because the tapered part of the tool is cutting the large corners, we should create these fillets first, before we add draft to the model. Then, while adding draft, we should select these filleted faces. This will give us a conical face with a taper of 3 degrees, to match the tooling we have in house (the tapered ball end mill).
After the large fillets and draft have been created around the perimeter of the model (which will become the perimeter of the main pocket in the mold block), we can create the smaller fillets at the top of the model. These will become the constant radius fillets which run around the bottom of the pocket, so the radius of these smaller fillets should match the spherical radius of the ball end mill.
As we can see, sometimes we create the fillets first and then add draft. And sometimes we create draft first and then add fillets.
This again shows the value of communicating with the mold maker. If we create the 3D model with a radius dimension or draft angle that the toolmaker does not have tooling for, it can significantly increase the cost of the mold and it can increase time it takes for the mold to be completed.
When creating 3D models which will become injection molded parts, we can save time and effort by communicating with the mold maker. We should be asking questions such as: “What draft angle (or angles) should I use for these parts?” and “What size fillets would work best for you?” We should think about how the mold block is going to be machined and we should use this to help determine whether the fillets should be added before or after draft is added.
In part 2 of this 2-part series, we will take a look at some other things to consider when designing injection molded parts.
Learn more about SOLIDWORKS with the ebook SOLIDWORKS 2022 Enhancements to Streamline and Accelerate Your Entire Product Development Process.