My CNC knife making thread

BossDog

KnifeDogs.com & USAknifemaker.com Owner
Staff member
I have always been fascinated by CNC machines. Put a chunk of metal in, hit a button and out comes your part. Easy peasy. 10 years ago I decided I would get one and make knives with it. This thread is about my experiences in working toward that goal. I'm not there yet but I'm getting close.

I am already full time in the knife business and it keeps me busy. Learning CNC and applying it was and remains one of the most difficult tasks I have ever taken up. It's no joke hard. I had no machining experience other than hand crafting knives. I came from a white collar career in retail with no exposure to manufacturing. . The guys that have done this on their own and making a living doing it are bloody geniuses in my book.

I will use this thread to document my CNC knife making progress and what I am doing or have done so far.
 

BossDog

KnifeDogs.com & USAknifemaker.com Owner
Staff member
I started attending classes 2 years ago at the local tech school 2 days a week. This included basic milling and lathe machining. Other classes included programming G code, engineering drawings, measuring, MasterCam and Solidworks intro/training. I am now 60 years old and was the oldest guy in the class and maybe the school. Most students thought I was faculty. College life is different than I remember it being. Anyway after two years of that I have license to learn. You will not learn enough in a 2 year machinist degree program to go out and run a business making knives using CNC. You will have to dig in and learn that anyway you can. I saw some students graduate with a machinist degree I wouldn't let operate my bicycle. The tech school route helped me get the basics down. Now I have to dig in and learn the details.

I watch lot's of videos' and subscribe to two different video training sites on CNC. I spend at least 3 to 8 hours a week now watching videos. I attend classes put on by the industry to learn more.


This is a HAAS CNC training class. You have a class setting with controllers at each desk. Students key in code or learn to use the controllers and then step over the machine set up in the class room. I have been to a 1/2 day on using the wireless probe and a full day intro to HAAS vertical mill. I have also attended a 2 day basic G code class.
HAAS class.jpg


This is my CNC machine fresh off the truck last August. It sat unused all fall as I had to concentrate on the business with the holiday rush. In January I started getting it fired up and now spend half of my work week and several evenings self training. Most CNC shops have specialists in several areas. You will have to learn them all. You will need to be the design guy that knows CAD and knives. I use Solidworks and have for years. I spent probably a couple hundred hours watching videos and doing training courses to learn it. It's expensive. There are cheaper options for CAM. Fusion 360 is OK and fantastic when you take into account cost.

This machine ran $68k. It has the wireless probe, high speed machining, network, air gun and couple other options. Tooling, vises were another $20k
HAAS VF2.JPG
Here is MasterCam training. 3 days of it. I have to sign up for at least 2 or 3 other Mastercam classes to even get through all the switch settings and options. Mastercam 3D costs $14,500 plus the annual maintenance fee is another $2k per year.
Mastercam class.jpg
 

BossDog

KnifeDogs.com & USAknifemaker.com Owner
Staff member
This is the first knife part I have managed to get out of my CNC so far. It is Ti and the lock side of a liner lock I make. I worked with a guy name Tyler to get this far. More about him later.
It's not much to look at but it's progress. I still have a business to run and that take the bulk of my time but I have made some changes here at work to give me more time to get this thing up and running.

First knife part.jpg
 

Smallshop

KNIFE MAKER
Tracy...great job!! A lot of guys our age hate the learning curve...but we're not too old to learn this stuff. I haven't used masterCam or Sw in over ten years. They are both great programs!

When I was a young toolmaker the "CNC guys" were making 3-5$/hrs more than a skilled manual toolmaker...I said nuts to that! Went to night school and took programming classes. Then I went and found a good CNC shop...I was a journeyman toolmaker at age 20...and a foreman in a CNC shop by age 24. I could learn quicker then...but fab experience is more important...my toolmaking experience helped me leapfrog over guys with years of CNC but no shop theory/principles.

Most seasoned knifemakers would make terrific machinists...manual OR CNC. Have fun!!
 

KenH

Well-Known Member
You're putting the time and effort into it - CNC stuff is amazing to me, even with my little desktop machine. It still uses the same Gcode as the "big boys" do.

Tracy - have you watched this video to see what can be done in knifemaking with CNC?
 

Smallshop

KNIFE MAKER
That is a good video. Aaron Gough's shop and tooling is very well laid out.
Tracy do you have rigid tapping on your VMC ? That was a pricey option on my first Fadal which I bought new in 2000. I went for it and about every job I did for the first few years had tons of tapped holes which made me glad I did. It's handy for knife making too...
 

Rick Otts

Well-Known Member
I hear wat you are saying Tracy I am in the process of learning CAD so when the time comes I can make flippers and test them on a 3D printer prior too making a prototype.I too have watched many hrs of videos and really enjoy yours you explain things real well.
 

BossDog

KnifeDogs.com & USAknifemaker.com Owner
Staff member
Today I spent a couple hours entering data into the tool crib in Mastercam. I didn’t care for the process that much but it was interesting in a way. Basically look up the technical data on all of your end mills, drills, reamers, forming tools, inserts, etc and enter dimensions (there are several per tool), SFM (surface feet minute) and FPT (feed per tooth or sometimes called chip load per tooth).

This all takes way more time than it sounds. I am starting out with Redline general purpose carbide AiTin coated end mills. I sent an email to my tool guy snarking about how much of a pain the Redline web site made getting tool data was. He calls me 10 minutes later offering to help. He was a good guy about it and talked me off the ledge.

My plan is to use middle of the road carbide tooling until I get some experience and then try some more aggressive feeds and speeds for fun. It is heart stopping to see a mill run full out using high speed machining. I want some of that.
 

Rick Otts

Well-Known Member
I believe some day there will be a easier way to enter data quicker.I was watching some videos on it last night with all the G codes man you need a book in hand to remember all that stuff but it was interesting.Wish I had the cash for something like that but they are out of my budget.
 

Smallshop

KNIFE MAKER
Tracy...building a "tool Library" will help speed thing up when actually programming. I have found the extra $$ spent on the high end cutters to not be worth it to me. I am not a high production shop so squeezing extra life outta cutter doesn't really work economically. I find that "middle of the road" tools like SGS and Mill Monster more to my liking/budget.

Some guys (like me) build their library the other way around. As they use specific tools and dial in speeds and feeds and depth of cut that actually work for them they save that to a "knowledge base" and then can access it by tool choices later on. Then it is "proven" data that worked on your machine with out doing so much up front data entry that might be tweaked later anyway. I'm not sure I have the patience to do all that up front...lol.

That interface looks real nice and streamlined to what I remember MC having. The last employer cam software I used was SurfCam...hated it in comparison to MasterCam.
 

BossDog

KnifeDogs.com & USAknifemaker.com Owner
Staff member
Currently I am researching tooling feeds and speeds and entering the data into my Mastercam tool library. This is less exciting than you think it is. It's a paper chase to track down SFM and Chip load (IPT) for each tool. Also several of my tools are just generic cheap carbide and don't have any reference data. Like a pocket knife, there is a HUGE variance in how each tool will perform. You'd think this would be easier.

I see now that I need to pick out a couple tool brands and stick to them. Lake Shore Carbide keeps coming up as recommended with several of the other CNC knife guys. I'll give those guys a try and then see what other brands will work.

Since I have no back ground in machining I don't have any experience to draw on to enter for depth of cuts, feeds and speeds. I bought Gwizard to help with feeds and speeds. This is a dedicated program to help give you a place to start with speeds and feeds by material and tool type. Gwizard runs $269 to purchase it outright or they have a subscription plan also. I'm not sure how well Gwizard will work with the optimized roughing tool paths Mastercam offers. We'll see. I guess I will run it and find out if I break tools.

After I get a handle on tool data I need to start looking for a repeatable pallet set up. A pallet allows you to clamp your parts in place on a plate - outside of the machine where it's easier and allows the machine to be running - and then put the plate into a vise of some type that is repeatable to .0005" or less. Pierson Work holding is a vacuum type candidate http://piersonworkholding.com/ that claims repeat ability of .0002"
 

Smallshop

KNIFE MAKER
Like a pocket knife, there is a HUGE variance in how each tool will perform. You'd think this would be easier.
LOL!! Yep....That was exactly my point in building the knowledge base "after the fact"....

If you already have a palletized machine ignore the next bit of info....If not, consider making double fixtures that will drop into your Kurt vises(Snap Jaw makes real nice step jaws that make this easy). pallets are nice for heavy jobs but for blades and handles probably not necessary.
On a new project here's how I begin my work flow. I build one simple fixture out of 6061 aluminum to prove out design. Then if it works well, I build a duplicate. Now I have two simple fixtures that I can rotate through the machine. While one is running the other is being unloaded and reloaded. As demand for product goes up (or a customers orders increase) I make the fixture bigger to hold more parts per operation. using the CAD geometry I will copy and paste multiples of the fixture I have already run and then re-CAM it.This frees up more time and also runs more efficient since the tool change time is always amortized by the number of part done in a given operation.
DSC01456.JPG
Here is the fixture I use on my little cowboy knife. It holds five blades and weighs 3.5 pounds fully loaded. it is 2" wide, 5/8 thick, 21" long...(read cheap to make) It takes about 1/2 hr to run the finish profile and 3 minutes to load and un-load. It I get to where demand gets higher I can make it 7x wider using 3/4 x 14 x 21 plate stock and run 35 at a whack and walk away from the machine for a few hours to do things like grinding, sheaths, cleaning, etc.

One lesson I have learned is that simple is best on fixture design. If you make an elaborate design you can become too invested in a so-so design that looks fancy thus resisting needed design changes. I love a tool that looks like a jewel...and I resist making them that way at all costs. Simple and accurate is the goal.

I've been job shopping on my own for 18 years...and have made some boo-boos along the way...so if I am over-sharing this is why...lol.

Hope this helps.
 

BossDog

KnifeDogs.com & USAknifemaker.com Owner
Staff member
Ted, I really appreciate the tips and pics. Keep them coming.

I will most likely start with aluminum plates and make some simple fixture plates dedicated to specific models. After I get good tool paths I will move it over to a work holding pallet set up to scale up a little.
 

BossDog

KnifeDogs.com & USAknifemaker.com Owner
Staff member
I am back to filling data into my Mastercam tool library. It turns out the cheap tools don't have published data like FPT or SFM and that makes it pretty much a guessing game for speeds and feeds. I am trying to avoid getting speeds and feeds by breaking end mills when I don't have to. I will have to look at picking out a couple tool brands that have testing data in a variety of appropriate materials and sticking with those. In the mean time these will get demoted to the manual mill for use.
 

Smallshop

KNIFE MAKER
I am back to filling data into my Mastercam tool library. It turns out the cheap tools don't have published data like FPT or SFM and that makes it pretty much a guessing game for speeds and feeds. I am trying to avoid getting speeds and feeds by breaking end mills when I don't have to. I will have to look at picking out a couple tool brands that have testing data in a variety of appropriate materials and sticking with those. In the mean time these will get demoted to the manual mill for use.
It might be easier to just run the formulas on cutters you have no info for. A rule of thumb is that roughing tools (Ijust use standard carbide tools...always 4 flutes) are going to be run at the lower end of the rpm range and higher end of feed rate (heavier chip load).

The formula for RPM is CS (cutting speed of a given material) divided by the diameter of the cutter x(times) 3.82.
So If I had a steel with "40" as the cut speed of material and was using a 1/4 carbide endmill it would be 40 divide by .25=160 x 3.82=611 rpm.

The chart below shows toolsteel as 100-300 using a carbide tool. If I average it I would use 200 as the cutting speed for a carbide endmill being used on toolsteel. You can baby the tools by going low on rpm and feedrate. so...200 divide by .25 is 800...times it by 3.82 (always a constant) and your rpm is 3056rpm.

But you still have to calculate feed rate to run. So you use the inches-per-tooth or what machinists call "chip-load" and calculate using the RPM you just figured out. So feedrate is the RPM times(x) the IPT (inches per tooth) times the number of teeth. So lets say your endmill has four flutes. you pick the column for 1/4" and you have .001-.003 allowable chip load on every tooth. So you go 3056rpm times(x) .002(middle of the road) times(x) 4(number of flutes) and you get 24.448 inches per minute as your feedrate. I always round off lol. F24.

Hope this helps. There are a bazillion charts you can find on the internet...as you most likely have. I find SGS a good middle of the road endmill...they may have speed/feed data.

Disclaimer...I haven't used this particular chart before, it was simple for illustration. A machinerys handbook(commonly called a machinists handbook) has most the
speed and feeds data in them. they are not cheap but worth owning...a ton of practical info there!!
tech-chart-speeds-end-mill.png
 
Last edited:
Top