There are several steps to creating moderately complex composite parts.
Step 1: Create your Design
This is the hardest part to the process! I typically do designing directly in CAD but a simple paper and pencil can also be a good place to start. Once satisfied with your design then draw it in CAD.
Step 2: Transfer the Design to 3D CAD drawings
The programs I use for CAD are Fusion 360 and Rhino 3D. Fusion works well for solid models and has the benefit of built in CAM. Rhino is better at organic shapes and complex surfaces. Use what you are most comfortable with.
For this demonstration, I’m going to focus on the nose cone for the RC flying wing glider I’m designing.
Step 3 Draw the Tools and Molds
With this stage of the process, you need to decide which parts you are going to mold. Once you have a list of parts, now comes the decision to machine the molds directly or make tool masters and pull molds from those masters.
There are several factors to consider in this decision:
- Machine Limitations that will be used to Cut the Molds or Masters
- The 3 axis or 5 axis CNC
- Accuracy, Repeatability, etc.
- Speed and Time required to machine parts
- Material Available
- MDF is the cheapest option but requires many extra hours of epoxy soaking, painting, polishing, etc and in the end is less accurate. Not very durable.
- Urethane Tooling Board – Most Expensive, fast cutting, very accurate, lighter than MDF or AL. Requires expensive sealing products. Not very durable
- Aluminum – Moderately expensive, heavy, and slow to machine, slow to polish, durable & accurate
- EPS Foam – Cheap to moderately expensive, fragile, fast to machine, requires extensive finishing work after machining. Great for very large parts.
- Solid Surface like Corian – Great for machining wing molds but only comes in 1/2″ sheets so requires gluing up layers to get a block. It’s also Expensive and very heavy but it does sand and polish easily.
- Mold life – How many parts is the mold going to make?
- How many sets of molds are needed?
Step 4 Create the CAM Tool Paths
For this demo, I am choosing to make a Male Master Tool of the Nose Cone and I’m going to use Reshape 440 as the material. The main reason I chose a Male Master vs direct machining a female mold is the limitations of the 3 axis CNC. Deep cavity parts with vertical or near vertical walls are hard to machine accurately on a 3 axis CNC. Also finishing a female mold is harder to polish vs a male master.
Creating CAM tool paths requires some experience with machining. At this stage you need also need to have a list of tools available, have decided on material as that affects how fast you can cut and how much per cut, know the feed and speed limitations of the CNC, and have some idea of how you are going to hold the part in the machine.
CAM is broken down into 3 main steps
Roughing Pass is used to quickly remove as much material as possible leaving just enough material that the finish process can easily clean up. Typically the idea is to use a big end mill so more material can be removed per pass.
For the nose cone mold, I chose a 1/2″ Carbide 2 Flute End Mill that I will run at 15K RPM. I use an adaptive tooling path to minimize the amount of time and maximize the material removal rate. I will leave 0.02″ radially and axially of material for the next step. Since I plan to use Renshape urethane tooling board material experience says I can cut this at 150IPM and take up to 0.75″ depth of cut in a single pass. I will climb cut vs conventional cut but either approach will work.
The most important check you can do is run the simulation and verify there are no issues. Once everything looks good, you can then post the tool path which creates a *.nc gcode file that the cnc machine can understand.
Finishing Pass I will break down into 2 different phases. First we need to use a 1/4″ carbide 2 flute ball mill to machine the curved surfaces of the master. To greatly reduce the amount of finish sanding required I chose a 0.002″ step over but it does greatly increase file size and machine time. Since I own the machine I don’t have to pay for time. I chose 12k rpm at 120ipm feed.
The Second finish phase are the flat surfaces and finishing the edges of the part. For this I will use a 1/4″ end mill with the same 12K rpm and 150 ipm feed rate. The step over is set to slightly less than the tool diameter to minimize the machining time.
Drilling Routines can be simple or complex depending on the design requirements
Here’s a list of the steps to drill a hole from a machinist perspective:
- Use a center drill or spot drill to locate the center of the hole.
- This step sets the location of the hole and ensures the twist drill in the next step doesn’t wander off position at the start of the plunge.
- Use a small twist drill to drill a pilot hole.
- Use the correct size twist drill to drill the hole (undersized of final required hole if using a reamer).
- Use a chamfer bit to de-burr the hole and leave a small chamfer if needed.
- Use an exact size reamer to finish hole to size.
- A reamer is needed if a accurate hole size is required. A twist drill will get you close but will usually produce a hole that is slightly oversized and sometimes not precisely round.
- Use a Tap to thread the hole if needed
- Manual tap is how I do it. Fancier CNC machines have the ability to machine tap holes.
For this part I chose to use 4 locating pins to help align the mold halves. I plan to use 1/4″ pins but at this point I don’t need to actually drill the holes so I am just going to center drill for the exact location I want. I will drill the holes later to size on the drill press and glue the locating pins in place.