We're expecting our machine sometime mid December.
5x12 flat table nesting, 20-something hp, 5-axis, 18+ drill block, ride along saw blade changer (up to 350mm)
We are (currently) 80% solid surface and the rest in plywood and HPL commercial and lodging case work with a bit of melamine here and there. Also, we currently buy a TON of MDF Doors so we'd like to start doing that in house (Raised panel for now and Shaker in the future)
With the CNC efficiency, we are hoping to start bidding every case good and millwork project we come across starting late spring so I expect our case good manufacturing to increase pretty steadily.

We are currently a panel saws / table saws, line bores, and routers kind of shop and have ZERO cnc experience. The manufacturer has sent a very basic starter tool kit with Fly Cutter and a few standard compression bits etc.
Additionally, we have a couple carbide insert VGroove saw blades getting fabricated.

My question is this - What tooling should I get , what tooling do you commercial shops use regularly? What tooling are you planning on getting?

I'd like to get as much tooling as possible before the Manufacturer install date in January so any input would be greatly appreciated.

Thanks in advance.

I don't have the answers for the best bits to use with solid surface etc. but can make some hopefully helpful comments.

You say "zero CNC experience". But does someone there have CAD/CAM experience? Bringing a low cost CNC into a small shop with no experience is one thing; doing that in a large commercial operation becomes questionable. There is a whole lot to learn beyond just running the CNC.

So assuming that the CAD/CAM side of things is not new to you then all you'll initially need to do is the (hopefully) included training session on the CNC upon delivery and setup. Looking at tooling in advance under this scenario is a smart thing to do.

As to the tooling, since I'm not experienced in specific tooling for solid surface and related products (I've only cut them a few times over the years and used my standard bits), I will just make some general suggestions. First, talk to your tooling distributor. If you don't get the kind of detail you are looking for there then take it directly to Amana, Onsrud or whichever manufacturer you prefer. They all have very knowledgeable tech people.

Then I will make one more suggestion based upon my early on experience. Don't by the most expensive bits initially. New to CNC equates to broken bits. It's better to lose the less expensive ones than the $100+ bits. I know this from experience with my first router where I was talked into buying a fancy 1/2" chip breaker bit. First, we ended up doing 90% of our cutting with 3/8" 2-flute downcut spiral bits (some even of HSS instead of carbide). Second, with the radius work we did in my shop we never needed the kind of edge finish you would get from a chip breaker bit, and third, that expensive chip breaker bit served as nothing more than a punching bag for all our learning mistakes. I was lucky that it kept breaking little pieces off the bottom.....i.e. kept getting shorter.......instead of snapping up by the collet which is often the case.

All of this was 25 to 30 years ago and much has changed in the interim. However I think these are basic lessons that stand the test of time.

BH Davis

You should be getting started on training on the software NOW, and worry about the tooling next. Any good commercial cutter company can get you started on tooling in a couple of days. It might take someone a couple months to be fluent on the software.

I am amazed sometimes at what shops buy. Based on your description of current work and future work, you should have at most bought a 4 axis machine, but regardless, for plywood, melamine, mdf, I would buy 3/8" 3 flute mortise compression bits. You will get good feedrates with a 3 flute versus a two flute. If nobody in the house understands chipload, please get educated. There are many calculators for that available for free. You can also build one in Excel. For solid surface, I use 3/8" diameter 3 flute low helix up spirals.. Those are excellent for glue joints and sizing. The mortise compression tools I mentioned earlier will allow you to do dados as well as thru cuts. If you can find someone to teach you programming and CAD/CAM, pay them to come onside, or online. You have a lot to learn. I've been doing this for 30+ years and still learn stuff from time to time. You have an exciting future if you do it right. I've seen shops with 8-10 year old machines and they still have no clue what they are doing. Good luck.

The necessary preparations include various cutting tools, clamping and fixing equipment, tool accessories, safety gear, maintenance tools, software, as well as training and consultation. Choosing the right tools and equipment for your workflow and project requirements is key to successfully using a CNC machine. Ensure that employees receive training and seek professional advice to ensure the safe and efficient operation of the production process.

happy to help with a starter pkg as we do it all the time, both for plywood, solid surface and all things in between.
have some tech white papers that can get you started in prep for your tech..
https://www.cnc-tool.com/technical-white-pages.html#/
my cell is 314-5041-8098
dylan

Oh sweet baby Jesus…

“ZERO cnc experience”

Sorry man, call that salesman and cancel that order.

5 axis machines are not made to run production SS, Mel, HPL, etc.

Obviously
They can. But it’s not even close to the best choice…..

Ugh. I’m sorry to be the Debbie downer but you’re in for a rude rude awakening sir. :(

What brand machine?

CNC's are a demanding mistress. Especially when you go more than 3 axis.

Your wife will likely start dating - the kids need a dad and all that.

20 plus years in this racket and learn/optimize constantly.

"What Manufacturer?"
We went with a Holzher 7535.
Flat Table with Outfeed.
Big drill block, 14 Changer (probably should have went with more), Ride Along Saw Changer.
Torque Lock 23hp Spindle.
590 Vac Pump.

I ended up getting our first run of tooling from GDP. The salesman seemed pretty knowledgable but he could have been just reading from a cue card. He was friendly though.
Bunch of standard bits he recommended plus a V-Groove Insert bit to compliment our V-Groove saw, a bunch of insert bits to do raised panel MDF, plus a pocketing tool and some other random stuff. He gave a "start up" discount of 25% so that was pretty clutch.

"Call the sales man and cancel the order. 5-axis aren't production machines"
Well, that's why I got a 23 hp spindle with automatic mechanical locking when working in 3-axis. Basically, it's just a weird looking 3-axis machine until I learn how to use its super power.

I mean, there are shops running production cabs on P2P machines. Now THAT seems like madness to me.

"CNC's are a demanding mistress. Especially when you go more than 3 axis."
Demanding mistress? Is there any other kind?
She's fun and exciting now, but just wait until I do the wrong thing and she has a full on melt down. Then nothing is going to make her happy but spending a shot ton of money on her. Yup, sounds about right.

I will say this, I am having a blast learning the software and about the whole cnc process in general. I chose to go with Mosaik and I am amazed at the capabilities. The learning curve seems pretty reasonable and I'm relatively sure that after the 10-day install/training and the 4-day software training course, and maybe a few hours of training with Mozaik, that I will be able to send basic, stock cabs to the cnc.

I had originally planned for 6-months after install before we'd be fully transitioned from our traditional methods to the CNC. But now I'm thinking it'll be significantly sooner.

You're going to run out of Mozaik pretty quickly with that machine.

Start looking at MasterCAM or AlphaCAM which I have.

"You're going to run out of Mozaik pretty quickly with that machine..."

For sure. Mozaik is just for the basic production cab stuff. I won't even use it for our countertops. It's way easier, for me anyways, to create the countertops in our drafting program and send them out as dxf.

I am currently leaning toward Solid Works (Learned 30 years ago in college and have since forgotten nearly everything) or Fusion 360 by Autodesk. I have a buddy who has Solid Works with Solid Cam so I'm trying to dig into that. Huge learning curve though, even with my past experience. Pretty much everyone recommends Alpha Cam so maybe I'll spend some time on some videos and see what I think. Fusion does seem like the most intuitive one I've looked at so far though. Although even Sketchup can be made to work for 5-axis with some file converters and gcode generators.

The Holzher machines come with NC Hops at the machine and I got a second seat for the Office. NC Hops for this machine has full 5-axis functionality plus it comes with collision detection and all that. My biggest concern with NC Hops is that there is almost zero youtube community in the states and everyone who uses it seems to speak German, so I'll be stuck trying to figure it out on my own.

And, if all else fails, I have no problem paying the nice fellows from India to provide me files all ready to send to the machine.

Congratulations on the machine purchase. That is a huge step forward from the basics.

As for tooling, look at what products you will be doing. Soon the tool changer will be filled up.
- Flat Panel: For routing compression and down shear should take care of most of your needs. This can be 3/8" or 1/2" with maybe a 1/4" for narrower dadoes. Also account for material thickness, bits with longer cut lengths will cut thinner material, yet is this justified by the additional cost?
-MDF Doors: The compression bit above can be used to cut out the door blank, yet all different tooling is required for profiled MDF doors.
-Solid Surface: This is a different set of tools. As noted you have a saw blade for inserts which I assume is for v-grooving. You will also need an up shear bit fro cutting out the parts. The geometry of this tooling is different than needed for the above. I typically use a 1/4" bit for cutting out solid surface.
-Drilling/Boring: Do not forget about this aspect of machining parts. Depending on the number of drills you can set up, try to find a happy medium between what is needed and the quantity of each bit. Boring is often overlooked when it comes to machining and time. Boring can easily take half or more of the time required per sheet. Standard boring is 5mm so you will want multiple 5mm bits in your boring head.

Software is another large factor in machining. There is typically better more useful CAM software available than what comes with the machine. I use Router Cim by Cim-Tech. This is AutoCad-based but is quite functional. If you are looking to do MDF doors, the software can set up macros, once this is done, then all the information the software needs is the size of the door.

You also mention Solid Works. It would be best to check into add-on software intended for the woodworking industry to get the most from the software. Do not underestimate the work that goes into making software work as you need. Also, if you are looking at Solid Works, I would suggest talking to Widom Associates, which offers Woodwork for Inventor. This is a good product that works inside of AutoDesk Inventor.

Lastly, find a tool supplier that knows tooling and specific needs for your industry. A supplier if issues arise or you have questions on which tool for a new material can give you a qualified answer. I use mainly Onsrud tooling, which has great support. You will get what you pay for in tooling, saving a few dollars, will typically cost you.

Best of luck on your journey.

Harry,

A long as you stay very realistic about the learning curve you will be fine.

A couple tokens of information I want to pass along from decades of running cnc routers at production volumes

1) p2p routers are great for horizontal routing/boring. Nested machines do not allow you to get to the center of the material (.375" above table). That's the entire reason for the pod system. This is even more a problem with moving gantry machines vs moving table machines. A moving table machine allows you to come in from the side where a moving gantry machine will always have difficulty getting to that location. (you may want to confirm that you have enough y-axis travel to get your horizontal boring heads to the edge of the table while allowing room for tool clearance.

2) 5axis machines are amazing machines. BUT for panel processing (countertops, cabinet components, sheet goods) They are not as stout as their 3 and 4 axis siblings.

I like to compare them to NFL running backs. A 5 axis machine is the best running back at the NFL combine. They have the best footwork, can jump the highest, and have the best training (technology). BUT this 5axis running back has very long legs and that moves the center of gravity higher and thus it makes them less stable.

3) Based on your products that you are manufacturing your spindle is drastically oversized. Solid surface cuts like a hot knife in butter with a faceted oflute. and 1 piece mdf doors take even less power. If I had to guess you'll be using around 6-8hp taking 1 pass cuts with a 3 flute comp cutter at ~1000 ipm. We have a 16hp komo router that absolutely blasts through 8/4 white oak with a 3/4" cutter and I'm at about 55-60% load.

Now having extra hp might seem like a great idea just to have it in case you need it? BUT with the added HP comes added weight. And ultimately more wear and tear on your machine and to bring the RB example back this 5axis RB not only has long legs but they are also very top heavy. So your rails, racks, bearings, and ball screws are under additional strain without any additional gain.

Software: This might be the absolutely most critical purchase to your success. I DO NOT recommend getting mozaik,aspire,sketchup,ect. You're going to have a lot of information to process and learn. And the worst thing to do is to spend months (even years) learning software that you will outgrow. Non of the companies use the same terminology or workflow so everything will be different when it comes time to switch to a more powerful software package. Do not cheap out on this. You're going to NEED training and a knowledgable support team.

Fusion
alpha cam
mastercam
Routercim/cimtech

Tooling:
other than some insert carving bits for your 1 piece doors. you're really only going to need a couple tools until you want to try different profiles.

QIC.tools has the best quality tooling and that's who we use for our primary tooling. They are the only company I know of that actually tests and provides exact %'s of cobalt in their cutters.

3/8" compression cutter
3/8" downspiral
1/4" compression cutter
1/4" downspiral

The tooling diameter is going to be greatly influenced by the amount of vacuum you're pulling. (which is not solely based on the vac pumps HP).

You want to make sure you're getting an MDF with the proper density level as well typically this is 38-42. Whoever your supplier is will have this information. and take special care in painting the outside of the board and ensuring youre surfacing both sides of the sheet.

Thanks a ton for the Info Z.
I just ordered a couple of faceted o flutes based on your suggestion.

"You want to make sure you're getting an MDF with the proper density level as well typically this is 38-42. Whoever your supplier is will have this information. and take special care in painting the outside of the board and ensuring youre surfacing both sides of the sheet."

Wait, what? Painting the edges and surfacing the spoil board on BOTH sides??
Does anyone actually do that in a production millwork shop? I have never seen a single youtube video in which the edges of the spoil board were painted and this is the first time I've heard of surfacing both sides of the mdf.

Remove the factory surface from the downside before milling the other up side. Painted or edgebanded sides? Nah, unless your vacuum is not up to the task. I have a 40 h.p. Travaini, so I dont have those issues.

our version of the best practice

https://www.cnc-tool.com/uploads/1/0/3/3/103363/spoilboard_applications_tips_sb-2023.pdf

Mike: your input was very helpful.... but actually not at all... i only suggested this since he is running SS and will not be covering the whole table.

We have a a csv151 40hp kaeser pump. I didn't realize this was a pissing contest??

Harry, youtube is not going to help... dont waste your time. you need to figure it out yourself and the best starting point would be the machine manufacture. Especially vac setup. there are quite a lot of variables that go into getting optimal vac hold down (table coverage, altitude, mdf spec, part size, etc

Z,
Not sure what you are even talking about. I was just saying that the factory surface should be removed from both faces. Standard procedure not matter what your vacuum h.p. is. Edgebanding or tape is only necessary for those with underpowered pumps or blowers. There are lots of vacuum pump options out there, so naturally there are different conditions in shops around the country. Altitude also plays a role. Trust me, I wasn't pissing on your leg. We are just offering some help if we can.

Hah. That went south real quick. I wasn’t doubting you about surfacing both sides, or trying to argue, I just couldn’t believe I was this far into it and had never even heard that the spoil board needed to be surfaced on both sides. But, sure enough, a few minutes on YouTube and literally everyone says you have to surface both sides. Anyways, I do appreciate the information. She just arrived this morning.

Harry,

I've been following this post since the beginning. I don't have anything to add, but I think you are on the right track and you are going to do just fine.

Mark