CNC Turning Guide

It's frustrating when dealing with sales representatives who have never touched a lathe and often give you a ridiculous quote. To better give an understanding and idea of what it takes I have written this page. 

Here are some basics to try and reduce the cost.

Insert Radius - On the tip of each turning tool is a super hard insert made of carbide, the bigger the radius the faster roughing and finishing. The insert will leave a radius in every corner, that is often assumed to be 0.032" unless specified. The smaller the radius the slower the machine runs in order to achieve a certain finish, also the weaker the insert. 

Grooving - A separate tool is required to make grooves, generally it's not a big issue on the outside of parts as it is the inside. The contact area of a grooving insert is quite large compared to other tools, so parts that are thin, long or flimsy will require a thinner grooving tool to combat tool chatter, caused by lack of rigidity. Thinner grooving tools means more machining time and poorer insert life. Internal grooving is considerably more difficult due to tool rigidity and groove depth. Grooving can greatly increase machining time and cost.

Threading - There are a lot of different threads, standard ISO unified and metric are often not an issue. Special buttress, mining and oilfield threads require inserts that are considerably more expensive, but with that requiring more difficult methods of measuring accurately. Internal threads require more tool rigidity, so deep bores require more expensive tooling. Smaller pitch threads have less contact area and therefore less chance of chatter. Thin, long and flimsy parts make threading more difficult due to rigidity. Large thread pitches make for extra difficulties increasing time and cost.

Drilling - Drills less than 0.125" diameter at a 5X depth become more difficult, the larger the drill the better stability and better coolant can get to the tip of the drill. I cannot drill more than 16 inches deep if the part can go inside my chuck, otherwise 8 inch depth is the maximum for parts 3 inches diameter or more. Drills generally don't bore an accurate hole with the exception of very expensive ones. Drills don't always go straight either, with the exception of buying special ones. 

Boring - Drills are used to pilot out material for boring which achieves better finishes and accuracies. Generally a boring bar can go to a depth of 3X it's diameter, exceeding this increases the risk of chattering. A 0.5" boring bar might only do a minimum o 0.625" in diameter at a depth of 1.5 inches reliably. There are exceptions to these rules such as anti-vibration boring bars that will do 10X depth. They cannot rough as fast and are incredibly expensive, for example my 0.75" boring bar cost me $2500. Undercuts are very difficult in boring, sometimes requiring multiple bars and special orientations of the inserts, adding to cost.

Knurling - There are a few different types of knurling tools. The older method is known as bump knurling which requires significant pressure on the part. If the part is sturdy then it's not a big deal, but it often takes a few attempts to dial it in, it also doesn't like materials too hard or too soft. The second is pinch knurling, this reduces the pressure greatly but the tool is less universal, it again doesn't like soft or hard materials. Cut knurling is the method I use, material does not matter and cutting pressure is minimal, it is however very slow. Knurling becomes very slow on large diameters, adding to cost.

Setup - The setup time is where the majority of time is lost, and while there are some standard tools that often stay in place, not everything is standard. Just changing the jaws to hold material may take 10 minutes, then 10 minutes to install and set each tool, and 10 minutes to make a custom set of jaws. There is also time taken to program the machines, manually requiring some thinking and punching numbers, or on the computer and drawing up a design. There is no such thing as a 10 minute job on a CNC. I do my absolute best to reduce this time, many shops will charge a 1 hour minimum for setup time alone. A part might only take 2 minutes to run but an hour to setup. So for a single piece it could be $125 or for two pieces $130,  so generally a quantity of 10 or more makes the most sense.

Tooling - Most turning can be done with standard tools, reading the above you can see difficult operations may require additional tools, something I don't have would need adding to the quote. There is also the factor of the insert wearing which is determined by material type, how hard it works and how long it works. The cost of inserts vary widely too, from $15 to $50 for turning and up to a few hundred for drilling. I make it the rule to charge $5 per hour of machining for steel and $10 per hour for stainless, that generally covers it, but sometimes increased if it's a more expensive insert. It is also the general rule to increase machining speeds until an insert breaks, with between 2 and 6 corners useable per insert. So if doing a run of multiple parts I'll charge $20 for an initial insert, if it's a one off then I won't.

This part is made from aluminum, it is 6.25" in diameter and 0.75 inches tall. It requires turning, milling and anodizing.

I first need to get a quote on material, since this is aluminum it often comes in 1 inch increments at these sizes. I must also calculate how many pieces I get out of a billet and how long the billets should be. Since the customer only requires 12 pieces I do not need to be as efficient with material, they also have a difficult feature and the material is expensive, so overall ordering extra is a good choice. Each piece requires 0.75" material plus 0.125" for the part off, plus a safety margin of 0.125". The length of the material I can place in my chuck is limited to 6 inches due to how long my drill is. The jaw depth is 0.5 inches, I require 0.25 inches for the parting tool and an extra 0.25 inches for safety clearance.

Ordering a 6 inch long billet will yield me 5 parts, I therefore need a total of 3 billets. I could of course reduce billet lengths to gain the correct amount with minimal waste, I could also reduce the length of the third billet, but again a safety margin is a good option. The material quoted was solid 7" diameter at a cost of $700 total.

The first step would be to turn the outside of the billet from 7 inches to 6.3 inches, then bore out the inside to 3.75 inches. Aluminum is often considered like butter to machine, in the way it likes to stick to tools. It can be machined very quickly if there is plenty of coolant, it can be a disaster if a tool gets gummed up. I predicted the billet setup and roughing to take 2 hours total.

These parts require an undercut on the inside at the back, while it is possible to buy a tool to do this it is unnecessary. The part still needs to be parted and then faced again to make that side pretty, parting doesn't leave a good finish like turning would. The face also requires a special groove, the tool costs $300 while a box of inserts costs $240. It would take an hour to setup and program a part. Each part should take around 10 minutes each, so a total of 2 hours to machine them.

Second op requires some custom jaws made to hold the parts gently and accurately. Around 30 minutes to make the jaws and $60 for the jaws. The second op faces the part to the correct height and makes it pretty. The large radius is then turned into the bore. I would figure an hour to do all of this.

Third op is machining a custom set of jaws for the milling machine and then setting it up, another hour of time. The holes are drilled and tapped, again another hour.

Overall it takes 120min (billet rough) + 60min (setup) + 120min (Op1) + 30min (jaws) + 60min (Op2) + 60min (Jaw+setup) + 60min (drill + tap) = 8.5 hours

$700 (material) + $300 (tool) + $240 (Inserts) + $60 (Jaws) + $1020 (labour) + $20 (Jaws) + $60 (drill+tap tools) + $100 (Anodising) = $2500

The tooling and jaws last an extremely long time on aluminum, so if the customer was to order this again then they would be paying $680 less, or rather $1820.

This part is about as easy as it gets,  turning the outside and parting it off.

The customer wanted a total of 600 pieces in S7 tool steel and 600 pieces in 4330V. The material supplied for the S7 was 1.25 inch diameter and 1.50 inch diameter for the 4330V. The finished part with a diameter of 1.239 inches and a +- 0.001" tolerance.

The S7 is a very soft material making it very difficult to achieve a good surface finish, by increasing the cutting speeds this is possible but at the cost of insert life. Due to the sticky nature it means the parting has to be slowed down otherwise it gets jammed with chips potentially breaking the tool itself.

The 4330V is a lot harder but an absolute dream to machine. There is a lot more stock to remove but this material machines very well by creating nice chips. It has to be run at half the speed than the S7 otherwise the insert would burn out. I can run the parting tool at triple the feed rate and rough the outside very aggressively, literally a single pass.

Surprisingly these parts take the same amount of time to make even though one has larger stock.

I quoted this job at 50 parts per hour which equates to $2.50 each. That leaves me very little room for error. I used an outdated box of inserts on this job that owe me nothing, but was getting 50 parts per edge, a little low. With 4 useable corners per insert that yields me at 200 parts per insert. In total I used 6 inserts for turning and 2 inserts for parting. The customer supplied me with material so I was willing accept this small loss. 

I managed to make 60 parts per hour on this job but combined with changing inserts and emptying chip strings every hour it averaged 50 parts per hour.

The goal in machining is to make material break into smaller chips, this is using the right speeds, feeds and insert. Depth of cut is also a major factor in this, so with the 4330V there was enough material to make it chip but not enough with the S7. The S7 left long strings which added to clean up time.

These are a bunch of 5/16" diameter studs with two different threads at either end, a quantity of 40 pieces.

I had the material supplied and cut for $53.

There are several options in turning these to the correct length, one would be to face one side along with the thread, then face the other side in order to measure the length, do some calculations and then place it back in the machine to face to the correct length and turn on the thread, this requires a lot more input. The alternative is to bunch all of the pieces together in my wire EDM, that way it can cut the pieces all to the correct length and removes one step of human input. It took around an hour to cut both ends.

I can then place them in the lathe with a stop so that every piece will be the same, but with this method I don't have to individually measure each piece and cut accordingly. One side is turned and threaded to 1/4UNC and the other threaded to 5/16UNC. 

It took me 1 hour to EDM the parts and then 2.5 hours to setup and turn the threads, so 3.5 * 120 = $420. Plus the material cost brings the job to a total of $473.