Desktop CNC router for plastic molds?

General Composites Discussions Composites Talk
#1

Does anyone here use one of those low cost desktop CNC routers to cut mold cavities in slabs of plastic or high density foam etc?

I am talking about those 3 or 4 axis devices that sell on eBay for between $300 and $1500.

I really dislike making molds by hand so, if possible, I would like to find a way to save at least some of the effort. I have found it impossible to find a CNC shop that would make some simple plastic molds for a price that makes sense for me. Most want to charge more than it would cost for me to buy my own CNC router so I want to see what my options are.

I want to use one to make two-part plastic molds for things like rifle stocks or bike frames. The max cavity size for my projects will be 24" x 7" and a depth of around 1.5" for each mold cavity (2" max for each half)

So, are people using these cheap desktop devices for make molds for cf or fiberglass parts?

If so, how many axis would be needed to cut a mold cavity in a slab of plastic for rifle stock or bike frame etc?

What sort of finish quality do you get? I.e. Are CNC cut plastic molds ready to use or do they require you to add additional gel coats etc, or a bunch of sanding?

How hard is it to use a CNC router? I am proficient enough in using cad programs like Maya and Mudbox etc, so I have the artwork covered. Is using a CNC router a case of learning how to use one new piece of software or do you need more complex programming skills etc?

Is a CNC router the right tool for making a small number of molds or does the set-up time negate any labor savings from making a mold by hand for low volume stuff?

If a CNC router is the wrong tool for a simple plastic mold, is there anything else I should consider?

I had my eye on a thermo vacuum forming machine. I was thinking to use my plug as a male mold and using a thermo former to make a plastic mold cavity around it. Anyone tried this or have a view?

I would really appreciate hearing from anyone with experience of using a CNC router for this purpose. I have searched on CNC forums but I can’t find any recent info that answered my questions and I really want to hear the answer from someone who makes carbon fiber products.

#2

The short answer to your question is yes, this is something you want.

Around a year and a half ago I built a version of an Open Builds OX which is an open source design based around open builds v slot extrusions and timing belts. It’s been super awesome and I use it regularly for do the exact thing your talking about. My machine has a usable area of around 1200mm x 800mm (48" x 32") and around 120mm of Z-axis clearance. This Z height lets you work in materials up to 50mm (2") though to do work on thick materials takes a bit of learning as the machine isn’t rigid enough when using a long end mill. I probably spent around $2000 on my machine but you could probably build something for around $1000

You would need a 3-axis machine for most of what you want to do. You can do highly curved and contoured parts with a 3-axis machine as long as there are no overhangs.

As for materials you can cut I have cut lots of MDF, plywood, blue or pink foam (XPS), urethane tooling boards, acetal and acrylic. For making molds your best bets from that list are tooling board, mdf and XPS foam. As for finishing the molds it varies depending on mold design, material and finish needed. The tooling board is great for what you’re describing but expensive. That said it’s dimensionally stable, machines super easy, and can, depending on the grade, be given a quick finishing sand and treated with a semi perm and it ready to go. MDF is much cheaper but is harder to machine, requires more work to get to pulling a part from the mold (though still going to be way faster then by hand) in most cases. This alone is a pretty big topic and there was a thread about making plugs and molds and almost all of what is discussed there is applicable to a cheap CNC

CAM programming is really just another piece of software. If you’re proficient at CAD you should be able to figure it out. A bit of trial and error involved but on a machine this size (or price…) the motors will stall before you can get in to too much trouble.

The CNC machine is one of the most useful machines you’ll also find yourself using it to make jigs and templates. Just don’t let your wife figure out what it can be used for or be like me with a house full of plywood furniture…

Couple of pics, one of the machine and one of a piece of MDF for a mold. The MDF piece was stacked on a stack of MDF rectangles to and covered with teflon release film to make a rotating bracket for a piece of electronics on Volvo Ocean Race 65. A good example of making something taller then your machine can handle by slicing it in to pieces

#3

You certainly can machine your own molds. The reason that pro shops want so much money is because it takes a lot of machine time to do 3d contouring. A large VMC costs many 10’s of thousands of dollars, and has operating costs.
The higher the quality you need, the smaller the stepover of the cutter has to be, and this adds a huge amount of time to the machining.

I doubt you will get a ready to go mold off of a machine without some handwork. The cheap cnc routers, because they are not rigid, will probably be far worse. The machines rely on a rounded cutter to step over and make a series of cuts to generate the profile. Generally there are little ridges between each step that need to be removed, the smaller the stepover, the smaller the ridge. It can take many hours to 3d contour even small parts. You only need 3 axis for molds like you describe.

Maya and Mudbox are art programs and I don’t think you can generate G code from the files.
I would recommend Autodesk Fusion 360. It is a reasonably priced (free for hobbiests) program that is true CAD/CAM. You will be able to generate G code from your drawings that the router will need.

Is a CNC router right you ask?, I guess the answer depends. It depends on the precision of the part that is required, the complexity of the part, your skills at CAD/CAM, and the quality of your router/mill to produce the part.

3D printing might be the next big way to make molds.

#4

Thanks for the detailed replies guys. They answer most of my questions in an extremely helpful way.

I dismissed 3D printing as an option because of the costs involved in a machine capable of making 24" long parts at a quality that is usable. I haven’t seen anything even close to suitable in the affordable desktop category. It sounds like a CNC router is the correct tool for my needs.

A few things I’m still not 100% clear on after reading the answers:

These ridges left in the mold surface that require hand finishing, how deep are they? I.e. Are they something that could be easily and quickly covered with a few coats of spray primer? Or are we talking about a rough sanding? If it’s the latter, it would pretty much negate all the benefit of using a CNC machine for me.

Surface prep of either the mold or plug is the thing that is most time consuming for me with a manual process. The mold surface has to be smooth enough to not spoil the surface finish of the carbon fiber parts.

If I understand the answers correctly, the finish level is somewhat dependent on the quality of the machine. I am specifically asking about the output from low cost desktop 3 axis routers so let’s assume it will be at the lower end of the spectrum.

If I import my cad files into something like Autodesk Fushion 360, are you saying that this type of software can output directly to the CNC router without me needing any type of programming skills?

The part I get confused on is that I frequently read post from people talking about “programming their CNC machines”. I can’t tell if they are writing actual code or if what they are really doing is the equivalent of clicking “print” on a desktop printer after selecting a few options?

If you have a finished cad file of a mold, how much work / time is involved after that before the CNC router starts cutting?

#5

I’ll quickly break down the programming and machining side which will give a better idea of what effects the finishing.

CAM (computer aided machining) programming can be done by hand for simple shapes. Most programming now is done with in a CAD program usually as a plug-in or in a stand alone application. There are a ton of options an most are quite expensive but there are some good cheap ones. I haven’t used it but I have heard good things about Fusion 360 as mentioned above which is free to students, makers and businesses making I think less than 100,000 a year and is cloud based. It’s also a full CAD program along the lines of Inventor or Solidworks so could also be a good chance to try a more technical type CAD program which can make designing some parts much easier. A good cheap stand alone program of decent quality is Estlcam. Plenty of good youtube videos about these programs. Probably the place to start is just watching some of these which will give you a good idea about the process.

Essentially the process is the same in all these. First you would define the stock essentially telling the computer what your piece of material would look like. You can often skip this step if you’re making a 2d shape cut out of flat panel. You then position the part in the stock. Next you tell the software where the 0,0,0 position of the machine is relative to the stock or part.

You have a selection of “tool paths” or “machining strategies” to choose from. There are simple 2d tool paths for cutting out 2d shapes where you would select a curve or edge and then define the cutting parameters. For 3d shapes you would normally use a “roughing” tool path which would focus on removing large amounts of material quickly and “finishing” tool paths for cutting the final surface more accurately. You would define areas with curves or by selecting face that you want to apply the various tool paths to and the software calculates the tool paths based on the cutting parameters defined.

The cutting parameters would consist of things like: step-over, cut inside or outside of the curve, diameter of mill or router bit, total depth of cut, depth of step down between each pass, speed of cut ect. This would be the voodooish part of the whole thing. While there are “feed and speed” calculators which help you figure out how deep of a cut, step over and the speed of the cut for various materials and cutting tools. Unfortunately these are more focused on numbers for industrial machines and hard materials so don’t always give numbers applicable to desktop or hobby machines. In the end with a machine like this there is a bit of trial and error to get numbers that work in the materials you use and give you the finish you want.

After creating the tool paths you can usually watch a simulation of the program which is always a good idea because it’s a free chance to catch errors.

The final quality of your mold will be a factor of:

  1. Material
  2. Quality of machine and tool
  3. CAM prorgamming

All the materials have different high points but to some extent the cheaper materials will have some higher cost in the finishing. Expensive tooling board is going to have sharper corners and sand easier than MDF.

Quality of the machine relates to the stiffness of the machine and the accuracy of the mechanics, ie amount of slop in the bearings and drive system. These factors also play in to how fast you can drive your machine and how big of cuts you can take. You might be able to take a deep cut but it causes vibrations which effect the finish of the cut. The tool should be pretty obvious but the quality, design and sharpness of your tools will having a effect on finish quality

With the CAM programming it comes down to a few factors. The first is choosing the right tool path for the detail and the second is the step over. Depending on if the surface is more horizontal or more vertical the different types of tool paths do a better or worse job of giving you a quality finish. The step over is essentially how far the tool moves between cuts. A very common finishing too path is parallel finishing. Imagine a series of parallel lines that are projected onto the surface of your part. The tool cutting edge follows these lines. The step over is the distance between the lines.The amount of material that is missed is determined by the step over and the cutter geometry. The smaller the step over the less finishing that will be needed but the more time it will take to machine. There will almost always be some hand finishing needed but the real time saved is in the getting to that stage and it will be easier to finish as the parts will generally be more symmetric and fair. The nice thing about having a small machine in a shop where it’s not trying to be used a direct income source is that if it takes a while it’s not a major deal. While you should probably stay in the area of your machine while it’s running until you have some confidence in your machine and programming skills it doesn’t require constant attention. If you come in first thing and start a part and it takes 8 hours so what?

The time it takes to do the programming varies depending on the part. If I need to cut out some plywood it might only take 5-10 minutes to draw the shape and make the program. 3d parts get a bit more complex but can also be quick, might be 10-45 minutes depending on complexity of the part and try to save some time ect.

The way that I would sum up my machine is that it generally does a better job than I can do in the same or less time. It’s definitely not perfect and I would never try to use it for production but as a support tool it’s awesome. There are limits on the accuracy but if you’re coming from hand made parts it shouldn’t be an issue.

#6

Nc42 gave a great summary of the process.

Just to answer your question above more specifically, you will need to do hand finishing. There are an awful lot of variables that go into the surface finish, but I would say that a $1000 router would get you the rough shape pretty closely. You would need to do a decent amount of smoothing to make a mirror surface- if that is what you are looking for. The biggest factors negatively impacting a cheap router are going to be rigidity, runout of spindle and resolution.

I have a 5000# Bridgeport Series II cnc mill (completely rebuilt) running a Centroid controller, and I could never get a finish that is ready for molding.

There are CNC machines that will produce a damn near mirror surface from the go, but you don’t really want to spend six digits on one.

I think that for making complex molds, CNC milling either the plug or mold is a huge benefit. You can make the part perfect in software, then have a machine make it so it only needs some smoothing out to be finished.

#7

Thanks. That is much clearer to me now.

I love it when I get quality answers from people who obviously know what they are talking about. It makes it much easier for me to understand and have confidence in what I’m told.

Does a mold cavity cut into a flat rectangular slab count as a 2d or 3D shape in routing terms? It seems like it could be either.

I think the logical next step is to download a few of these programs to see them in action and then, once I figure out how to use one, maybe I’ll rent some time at a local maker-space to see if I can give one a try.

I was thinking to make my own tooling boards out of epoxy putty. The one I use most is rigid but the surface hardness is more medium than hard, so it’s less harsh on router bits. It states that it’s suitable for CNC routing in the data sheet. More importantly for me, it sands easily and can be polished to a glossy finish without much difficulty.

I should also look at some of the coating that are sold to smooth 3D printed products. Perhaps they have a labor saving application for CNC cut mold cavities.

What determines the resolution of a CNC router? Is it the controller, the software, or the spindle?

#8

If the part can be cut with simultaneous X and Y movement, then it is 2d. 2.5d would be when the Z axis moves, but not simultaneously with the X and Y. 3d would be when all 3 axis need to move simultaneously to perform the cut- the machine can move the cutter smoothly in 3d space.

Your machine resolution is going to be determined by the controller, the drive motors and the feedback (or lack of). Higher end CNC machines use linear encoders that are the travel length of the axis. These linear encoders provide the control with a highly accurate position of the cutter at all times. Less expensive machines would use rotary encoders on a servo to provide feedback. The rotary encoders don’t guarantee the position at any given moment like the linear encoders, but are highly dependable. Steppers have no feedback at all. Steppers work well, but their resolution is much lower than a servo and there is a chance that they may miss a step. It is common to use microstepping when driving stepper motors. Many people think that it increases the rotational accuracy of the motor, but it does not. The microstepping enables the motor to spin smoothly and not in a strongly pulsed rotation as would occur if not microstepping.

Drive reduction plays a part also. Having a high resolution drive motor is not going to help out when your leadscrew or belt drive has backlash in it.

Of course, all of the above you can throw out the window if the machine is not rigid enough to take advantage of a high resolution setup- which is probably why steppers are used on the low end router tables, along with the fact that steppers are cheaper to purchase and drive.

#9

Some of my mold cavities have 45 degree angles. I was trying to understand how these cuts would be made on a 3-axis machines. I had it in my head that the angles would be cut using lots of linear horizontal cuts at multiple heights and that was what caused the problem of these ridges mentioned above.

I guess it makes more sense that the angles would be cut with a simultaneous xyz motion. This would make some (but not all) of my molds 3D.

Am I right in thinking that the controller and the motors can be upgraded at any time? I.e. If you start with a cheap machine just to get used to it, you can upgrade steppers to servos, buy a better controller and maybe even longer rails to get more cutting space?

I realize that if you upgraded all that at once, you might as well just build a whole new machine.

It looks like most of the desktop machines I can find on eBay that can cut 24" mold cavities are 4 axis. I was hoping to save money if I only needed 3-axis…

Maybe it’s best if I try and do a diy build so I can get the best of what I do need and not waste cash on capabilities that I don’t.

If making the machine as rigid as possible is a major concern, have any of you tried replacing any aluminum and wood frames with carbon fiber?

It seems like reinforcing the frame would be an easy diy job.

#10

For the size you are talking about I’d look at http://openbuildspartstore.com/c-beam-machine-xlarge-mechanical-bundle/. There are a number of controllers that could match with this. This is probably the best machine you can get for under $1500 which is about where you’ll be once you add a spindle or router and a controller. It’s also easy modified to give you more z height or make other changes and has a large community in the open builds forums.

Adding carbon can help, if you look at the picture of my machine I have carbon reinforcement on some of the axis. On the normal version of the OX the X-axis is made from 2 20mmx60mm extrusions. On my machine I glued pieces of 3mm c-plate on the outsides and in between the extrusions. It definitely doesn’t hurt… That said stiffness is only one part of the equation so a pure carbon machine isn’t necessarily better than an aluminum or steel machine.

#11

I have a large 5 axis router that we use for both production and pattern making. You asked about the quality of the finish and has been explained, better than I could, there are multiple factors that go into the quality of the finish. There is a balance point between machine time and hand work that can be hard to pin down without some serious consideration.

I’ve recently done a little study to see where the best bang for the buck is for us. I considered three types of material and factored in machine time, hand work, and end use.

As far as machine time goes, as was stated, if you are confident in your program and have the right equipment, you can start the machining process, walk away and do something else while it runs, then come back when it’s done. I’m working on a design right now that might take 20-22 hours to run. Our machine has an automatic tool change capability with a 12 place turret so I have a variety of tools I can use to get the best surface possible. I will probably run the program over a weekend - like Ron Popeil used to say in those late night infomerrcials - “Set it, and forget it”. I could set up the program to run faster but I’d end up with more hand work. If I needed the machine for production on the weekend, running faster would be a factor in that decision.

Hand work can be a variety of things, from merely polishing the surface to applying additional coatings and fillers.

As for end use, I look at what I am trying to accomplish with the part coming off the router. Is it a on-off buck that will be laminated as an end product? A pattern for a mold? Perhaps a pattern for multiple molds in a production setting? Maybe you want a direct mold for a limited production run.

For materials in my little study I looked at 12 lb density urethane foam tool board, 28 lb urethane foam tool board, and 71 lb solid urethane tool board. At my current pricing, for 2" thick material, the cost per square foot is $12.56, $19.70, and $56.24 respectively . What I found surprised me to a degree.

I’ve been using 12 lb for quite a while but I’ve never been completely happy with it. The cell size is such that it takes a ton of primer and polyester spot putty to fill the resultant pinholes. My basic approach is prime with Duratec Surfacing Primer, fill, 150 grit sand, prime, finish sand. As you can guess, it’s a lot of hand work time, and care must be taken to retain detail and tolerance.

I decided to look at higher density materials to try to reduce the hand work. I was talking to my supplier about the 28 lb material and he suggested to also look at the solid, 71 lb stuff. I figured this would be outrageously priced and I wasn’t wrong about the material cost. I got some samples and played a little and found some interesting things.

The 28 lb foam requires a single prime coat and a few spot fills at seams so it finishes out much quicker than the 12 lb. The 71 lb stuff doesn’t require any primer so all it needs is finish sanding and polishing. This made me sit down and exercise my brain a little.

The conclusion I came up with is the 12 lb foam is good if you’ve got more time than money. The 28 lb, although more expensive than the 12 lb, is actually cheaper in the long run if you are paying for labor. The real surprise came from the 71 lb stuff. If you are building multiple molds (as we do) and want a permanent master to pull those molds from, the 71 lb urethane is the way to go. Instead of building a pattern and then a mold and then pulling a master from the mold, you go direct to master and then mold your production sets off that. I figured it’s about 10-12% cheaper and time to market is about a third in our case. This info is for relatively small items. It might not pencil out for something like a boat hull or a airplane wing.

The 71 lb urethane can be polished to a high gloss if you desire so you could make a direct mold from it and polish it to your requirements without any primers. I’m attaching a picture of a direct mold set I built as a test. It is a structural, non-cosmetic part. The male part was only sanded to 600 and hit with a quick buff. The female part is right off the router.

#12

I have various urethane casting resins on my shelf (as well as other types), I could probably make my own tooling boards to save money if needed.

Have you ever tried making your own tooling boards from a 2 part resin? I have various ones that state that they are suitable for CNC routing.

I also want to try using Free Form Air epoxy putty to make CNC tooling boards because it’s so light, strong and cheap. It sands / polishes to a relatively high gloss fairly easily.

I noticed that one of my (soon to be) competitors seems to use wood for their tooling boards which they coat with a gel coat. It wouldn’t be my first choice but they are the largest company of their kind so I guess it can work…

#13

Thanks. That machine looks perfect for my needs. It’s much cheaper than anything else I have seen in that size.

#14

I am just getting into this area myself for hobby builds. These will be small (10 inch x 6 inch or less) and very shallow (0.25 inch or less) parts from half molds using carbon cloth and tow that are RC sailboat rudders and keel fins, so while they are somewhat structural, no ones life depends upon them :wink: However, it is important that they have an accurate profile - more accurate than you can make by hand - and they have compound curves so must be cut with a 3-axis machine.

If you are going to do just a few parts and are in a larger city, rather than build your own machine, see if there is a local “maker space” - sometimes call a hacker lab you can join. The local one to me that I will be joining ($100 USD/month) has a 48 inch by 96 inch bed ShopBot that turns out pretty good parts. This has the added advantage that in addition to the machine, you do not have to buy the CAD or CAM software which is very expensive. There are free open source programs (TurboCAD is one example), but most do not have an easy to learn user interface. Fusion 360 is free for hobbyists but it has a complex interface. The Vetric Software program VCarve Pro, is super easy to learn, but costs $700 USD, so you can see the difference. Some packages are up in the $2,000 USD area. Most programs offer free trial downloads that cripple the file saving or allow a limited number of saves so you can test drive the program. If you do build your own machine, selecting a CAD/CAM program that has lots of YouTube tutorials is a big help.

Depending on how busy the machine is at a hacker space, you may have to sign up for time, but many are open 24/7. This is not a great option for a production environment, but great for a hobbyist like me.

As far as materials, the hobby RC airplane guys use MDF to mold their wings. They do a rough cut, remove the mold, coat it with thinned epoxy catalyzed resin, let it cure and then put it back in the machine to do the finish cut. If you use polyester resin rather than epoxy and do very small step overs, the finished surface can be lightly sanded (600 wet up to 1500 wet), cut and then buffed to almost a mirror surface - not as reflective as an aluminum mold, but very good.

Another thing to try for the material for small size molds is Corian or any solid surface counter top material. When milled with a 0.125 inch ball end solid carbide three flute up cut bit and finished, it makes great molds for limited production run parts. You can usually get sink cutouts of the material from the local kitchen and bath cabinet builders very inexpensively - like a dollar or two each, since they would throw them away.

There is a good forum on CNC things in general at www.cnczone.com, including threads on home building your own machine, including the people who are currently making the best kits. Do some reading there before you settle on a specific machine to build.

Good luck. It is a long but interesting road.

SS//

#15

I’ve decided to have a go a building one myself. The advice I’ve been getting is that it’s pretty much the only way to get what I need from my tight budget.

It’s amazing how much the price goes up if you have somebody else do the shopping for a parts kit.

I have started ordering parts so we’ll see…

I am very curious to see if one of the open builds single board CNC controller / cam software / stepper driver will do the job I need. If it can, it will be a huge saving. The saving looks so large that I’m convinced there will be a “gotcha” in there somewhere…

#16

There are so many boards to choose from now a days… which one did you buy?

I’d like to see your final BOM for parts and the total cost.

We bought a shop sabre 3 axis cnc, it was about $20k, a bit more probably… I’d think that one could be built for less. It uses the Win CNC controller.

#17

I haven’t 100% decided on the electronics yet but I’m close to pulling the trigger on a Gecko G540.

I have already ordered 4 Nema 23 high torque stepper motors which I got for $100 for the set. I have also bought some of the rails. I bought two 1000mm THK 30mm rails with four bearing blocks for the X-axis. I got them used for $150. I got a 1/2" two-start ball screw with all the necessary blocks, bearings, couplings etc for $30 (also used).

For the Y-axis I bought 20mm THK rails (600mm) with 4 bearing blocks for $70 for the set.

That’s as far as I got. I’ll probably order a generic 2.2kw spindle off eBay for $250 with the inverter. I already have a bunch of spare power supplies and desktop pc workstations here so that part is taken care of. I plan to make the frame components myself from carbon fiber.

I don’t know what the final total will be but I’m positive it will be nowhere near $20,000. I’m guessing your machine is a much more serious and impressive piece of kit than what I’ll end up with…

#18

I think you’ll find that the 2.2kw spindle is actually overkill and the weight of it will be a negative. I have a 1.5kw air cooled Chinese spindle on my machine and machine rigidity becomes an issue long before the spindle is unable to cut. I’ve started running 1/2" router bits with a 1/4" shank in it which speeds up roughing quite nicely

#19

Here’s a deck plug for a model boat for a friend I cut last week. It’s about 900mm x 300 aft the stern and 50mm deep. Took about 5 hours with a .6mm step over pin the finishing pass which means not much sanding to finish it.

#20

sorry for giant picture…