I’ve spent considerable time researching System32 templates that are used with hand-held routers to drill shelf pin holes, assembly holes, and holes for System32 hardware. The two that are at the top of my list are the Festool LR32 system and the Schmitt32 system. Both are spendy, accurate, repeatable, and reliable. It doesn’t take too many ruined cabinet panels to make the price of these two systems seem pretty reasonable.
Then there is a third option - CNC! I’ve read several articles that warn against drilling holes with a router. Heat buildup, inadequate chip removal,having to spiral or peck the holes etc. What seemed like a great idea just a short time ago now appears to be a disaster in waiting.
Does anyone here have experience with this process? If you’ve been successful, how have you gone about the work? Bit selection? Straight plunge? Spiral? Peck? Feeds and speeds? RPM? If CNC really is a poor choice for this application that’s fine. I’ll go with one of the other solutions.
I appreciate your willingness to share your expertise!
I’d wait to see if someone with experience of both can comment but looking at the demo systems I can not imagine you’d have a different drilling performance, looks like LR32 uses a router, set up time looks like it might be comparable (or even quicker with the 1F, using x and y guides with known positions.). I’ve drilled holes with the 1F (my first job whilst making the waste board) but not into melamine veneered chipboard.
You can ABSOLUTELY use a CNC to drill holes and build cabinets, its what the big mill shops use to cut theirs. I’ve done peg shelving pins in my cabinets using the OF and they come out 100% every time.
However you DO want to use either an Up-Cut bit or a bit made for drilling. While you get a really smooth cut with a downcut bit, the smoke and burning you are talking about are from that chipload not having anywhere to escape and just being heated with friction until it smokes.
Thanks, Andy. It seems that CNC bits for smaller holes (5mm and 8mm) and the high speed of a router even on its slowest setting, are thought to create so much friction in any wood material that the holes glaze and burn. The odd thing is that both the Schmitt32 and the LR 32 systems use a router. I’ve also used similar but non-production systems in the past and have not encountered burning. Bits sharp, of course. I also wonder if those commercially available pre-drilled cabinet panels are made with CNC or with big line boring machines. Probably the latter.
The Festool and the Schmitt32 are expensive - a frivolous purchase if the Onefinity can handle the job efficiently and effectively. I have an ocean of cabinets ahead of me, and the right decision is important! We’ll see what others have to say. Thanks again for taking the time to respond.
I had the LR32 system and found it too fussy and time consuming to setup and use so I ended up selling it. I love my Festool but that one just wasn’t worth it for me. I will probably try using my 1F for pin holes once I get a cabinet job to justify it. Until then I’ll just use my Kreg shelf pin jig.
Bit selection is key. A 1/8" upcut endmill with a spiral drilling operation (I know that’s an option in VCarve, not sure about others) works well. There’s also a 3/16" special endmill I have that has an offset tip (vs a flat end) that is designed for drilling with a CNC. I expect something similar to that is used in a lot of commercial operations.
Conventional drill bits aren’t designed for the speeds of a router. There might be some rated for 6K+ rpm but I haven’t looked. Amana or Onsrud or Whiteside would be where I would go looking though.
Hi Jim, Your worries of drilling with a router are unfounded. The two template systems you mentioned use routers as well, so its not the router that is the issue. Its the setup and bit that you use. If you use the upcut spiral bit designed for routers with the correct speed you will get good results. The Onefinity, along with good software, (VCarve) will set you up for the fastest, most accurate, and repeatable hole drilling that you are looking for. Once your program is set up and tweaked the way you like it, you will be able to repeat the process over and over again letting the machine do all the work eliminating any human error in the process.
I understand that conventional bits are not part of the equation. I do have VCarve, so spiral drilling is a possibility. I’d have to get a bit something a little under 5mm and another a little under 8mm. Jim - you have had luck with upcuts? No fuzzy edges in wood or plywood, and no chipped edges in Melamine? I get the need for chip ejection, though I have traditionally used downcuts to get clean, sharp edges.
I actually use compression bits for my go-to bit choice. You have to drive them more aggressively so you get the up-cut portion (it’s about 1/3 of the length) into the material right away and the down-cut into the wood. They’re really good for melamine to get clean cuts on both sides. The 1F is sturdy enough to handle the deeper plunge of a compression bit - just use good ones that are sharp.
I would try using several bits on a trial run to see which gives the best result in a given wood. Also try different speeds and plunge rates for the best results. Use the advice of others as something to try, but do your own testing to get the results that you want. My advice is to use an upcut bit, maybe even try a four flute upcut bit with a moderate spindle speed and a slow plunge rate.
Hey there, I have successfully drilled about 1500+ 1/8" holes for crib boards. I set the router at the lowest speed, drill to the depth of the flute length with a spiral upcut bit. I havent had any issues.
I was super worried about all the things people mention but drilling 373 holes per crib board by hand sucks, and if the bit doesnt get optimal life. I dont really care.
What I have noticed throughout the CNC progress is its all about chips. You want chips and not sawdust, if you find a recipe that produces chips youll be alright. In most of my cases its the work holding that is the limiting factor on how aggressive I can be. And I will trade reliability for a few less hours of bit life any day.
Depending on your hole size, if you can bore youll be good. And if need to drill you will be fine. The limiting factor will the be the flute length and whether or not that is long enough for your application.
Drilling gables with the Onefinity CNC is a game changer. It works great! You can drill whatever pattern suits your needs best. By setting up so shelves can be mounted verticaly at the front, you can drill dowel holes. The matchup between the gables and shelves is perfect.
I have my gables set up to drill all hardware holes, dowel holes, and a blind dado at the back for insetting the back.
Saves so much time and moving parts around over and over for different operations. Plus, you can do something else while your panel processing is running.
Recommend this machine highly for your application
Thanks, everyone. This has been informative (!) and encouraging. I now have a very good idea of the formula for success, and that success can indeed be had given a little patience in dialing in bit, spindle speed, and feed rate before starting production. Fred, you have me stumped. What is a gable (other than that at the top of a house)? And Fred, you are cutting your cabinet sides to size and them using the OneFinity to do your 5mm system 32 holes, your 8mm construction holes, and your 6mm back groove? If so, would you mind sharing how much time each panel spends under the OneFinity?
The gable is the correct name for the cabinet side.
You can forget about “system 32” as you can locate the holes wherever you want. Nothing really works well on system 32.
I use a vacuum clamp. Just made a special spoil board with holes placed in the right places so different size gable will still fit. Just using my Festool vacuum.
With no clamps, the clearance height can be set to 2 mm, saving a lot of time.
Each gable takes about 5 minutes. Spindle speed 24,000, feed rate 3000 mm / minute. Single flute 4mm dia cutter. The dado at the back is 16.5 mm wide x 2 mm deep. So 16 mm thick back slides in.
Tried to answer your questions first. Getting back to 32mm system. I discarded that years ago.
Here is my system. Base gable is 767 mm high. Subtract 5 mm for a little clearance between drawer front and countertop.
Now picture 5 drawer frontsneeding 3 mm space between each front. Subtract 12 mm.
So now you have 5 drawer fronts, each 150 mm high. 3 mm space between them. 5 mm space at the top.
Pot and pan roll outs, add 150 +3+150 303 mm high front. And the 3 mm space lines up with the adjacent cabinet. You can do lots of configurations and the space between fronts lines up with adjacent cabinets.
Looks great, but does not conform to 32mm system. But with the OneFinity, you can drill your holes wherever you want. 32 mm system was invented for line boring machines with multiple spindles with cutters spaced on 32 mm centers. No such requirement anymore.
Table is set up for other projects now and did not want to replace spoil boards.
you can see the clamps for vertical panels.
Pic1: Under this spoil board, in the main table, i used onefinity to drill alignment dowels and to cut the slot at the front of the table.
Pic2 shows the vacuum table. It drops down over the dowels and the front edge aligns with the table slot. (both cut with OneFinity, ensuring accuracy and fit.)
Squaring brackets were added under the table.
The drawers underneath can be pulled out and support panels at different heights, with shims.
The vacuum table holds one base gable or varying heights of wall gables. Gaps need a panel inserted to stop vacuum leaks.
With no clamps, I set clearance to 2 mm, saving time on machine movement.
Pic3 is my cheat sheet for door heights and widths. I try to keep to standard sizes, but easy to change if necessary.
