CNC Routing Aches and Pains - Machining Methods/ High Volume Wood Porduction??

Hey Guys,

First-time poster, but hopefully can generate some good quality information from this.

Soo my this is where I am at.

I purchased a Biesse Rover J Plast a little over 4 months ago. I had a purchase order of 5,000 units of a product I designed. 5,000 units equaled to 25,000 finished CNC cut parts. 10,000 of those parts were from 9mm Hydrotek Marine Plywood and the remaining 15,000 units were out of 6mm Hytroket Marine Plywood. My shop is at around 6,000' of elevation I'm running 2) 25HP Becker Pumps paired with a 10HP (24000RPM HSD Spindle). My first issue arose with finding the correct spoil board. After many and many attempts, I settled with Ultra Light 1" MDF. This seemed to give the best hold-down and lasts until I get to about 1/2" thickness. PVC Edge banding.

Secondly was getting my feeds and speeds correct. I ended up purchasing GWiazrd and used their calculations. Needless to say, I burnt up my spindle in roughly a month and a half. Biesse said I was crazy for running my spindle close to maxed out, but the salesman said it will do 24k all day and night. Either way, the spindle was replaced by warranty. I'm reluctant to spin this above 22k now, but I suffered in completing this PO of 5,000 units, but it's finished. Now I have a PO of 20,000 units!

I'm back to testing and figuring out the best machining methods. I've purchased a second CNC to cut my 1,100 man-hours of routing in half. I'm not purchasing another Biesse. I was promised that it would not have any limitations, but only benefits from their processor. That is most assuredly not true on their 3 axis routers. It was complete and utterly a pain creating a post for fusion360 for this controller. If I did purchase another Biesse my post wouldn't work either so it's completely out of the question. Long story short I'm getting a machine that reads standard G-code with the same hardware specs.

Now back to testing, I'm finding that with my nested parts which range from 54-88 units per 4x8 sheet that I'm burning up bits in 2-3 sheets. I run as little as 7 sheets a day. In comparison to a cabinet shop, I'm doing enough cutting in a couple of hours than most see in a week. I've tried multiple different methods from slower to faster/ multiple depths/ doing a larger diameter to a smaller diameter in multiple passes/ all seem to dull bits at about the same amount of time. If the bit gets dull then my employees are sanding for the next month and it's moving my parts. So, in short, keeping my bits sharp seems to keep the operation as smooth as possible.

I've been using
Armana
46398-K 1/8 mortise compression
46200-K 1/8 down cut
46029-K 1/4 mortise compression
46181-K 3/16 mortise compression

Vortex
3115 mortise compression

These are my most recent test bits. I've used almost every other Armana bit out there that matches my type of cutting with the same results.

Sharpening bits seems to be out of the question because after my 2-3 sheets the hook on the end of the flute is basically sheared off. I have recently heard that all bits are meant to last for 15min of solid cutting. I do this in less than 20 min of my workday.

2 of my parts require hidden pocketing as which I need a router for. These 2 parts are the most time consuming and adds up to about 800 man-hours. The remaining parts are smaller and just need to be a 2d through-cut. I may switch to a laser cutter for these parts to eliminate the bit issue, moving part issue, headache, and be able to cut these parts in line with the router for reduced timing
.
As I said I am new to matching. I've been at it for 4 months and have overcome many hard-learned lessons, but I am still learning each and every day. I feel I have exhausted every contact I know. Most of my contacts that machine are primarily geared towards metal so their input has helped, but I've surpassed what they have been able to offer and now I'm strictly into the testing of high volume production with wood materials with machining methods.

The reason for this post is to generate any helpful knowledge I can pull from this user forum. Please don't hold back and give it to me straight.

Best,
Jake

What feedrates and RPM are you using with each bit? With a 1/4" bit, you should be able to get close to 500 ipm with a 1/4 bit at 18,000 rpm. But if you're cutting small parts, the machine may not be able to ever reach very high speeds.

It sounds like you have a combination of the most difficult things to route. Small parts, that require small tools, with a very abrasive material.

You want to run as fast as possible, with the lowest rpm, without the tool breaking, and maintaining acceptable cut quality.

From my experience on big machines (I use a Morbidelli), Amana bits don't compare to Vortex or Onsrud. Shorter life, and much poorer performance.

Smaller tools wear out much faster than larger tools. If you can use them, you'll get considerably more life from a 3/8" diameter tool vs a 1/4" tool.

If possible, I'd remove most of the material with a roughing spiral, like a Vortex 1140. Then just do a light finish pass with the compression bit, and it'll last a LOT longer. And if you can use them, the Vortex XP series can last 5x longer.

Hey Gerry

Tool 3115 - 18000RPM / 2403.5 mm/min / dulled in 3 sheets
Tool 3112 - 18000RPM/ 11887.2 mm/min / dulled in 5 sheets
Tool 3115 - 20628RPM/ 7880.0 mm/min / dulled in 4 sheets

Currently testing
Tool 46181-k - 18000RPM / 8000/ mm/min / on 3rd sheet frying starting to show.

When I say dulled the parts at that point need sanding.

So far running the feeds faster and slowing my spindle speeds seems to be yielding longer life.

I cannot use any tool for these parts that's bigger than 1/4" due to design.

Best,
Jake

Its the adhesive used in ply manufacture that typically kills all tooling. I have no experience with Amana or Vortex in a production setting, but the folks at Onsrud (LMT, Leitz) will knock themselves out optimizing a tooling/material match. Your application may also be a good match for diamond tooling (I have no experience here). What I understand is that poor quality board kills diamond tooling. Read the industrial specs for man made panel stock and look for grit content. It includes fly ash, grit, gravel, etc. (typically for particle board, mdf, vafer board). It is hitting very hard objects (or dropping tooling on concrete floors) that do in diamond tooling.

Yeah, most marine ply is coming from overseas. Really hard to tell what's in it and how it's made, but the filler is what's killing me. I've reached out to Onsrud to see what they can recommend and do. My main issue now is finding 1/4 or smaller bits that offer the same types of profiles as the larger bits. In hindsight, I would have designed this a bit differently.. too late now :) Maybe come out wither version 2.0 later next year if orders keep increasing ><

Tool 3115 Vortex - 17000 rpm/ 12000mm/min a/ dulled in 7 sheets (this takes about 17min per sheets)
Tool 46181 - k amana 8000RPM / 8000/ mm/min / dulled in 4 sheets.

Have you tried an over-material rough cut, followed by a cleanup cut with a separate cutter? I use a 3/8 DS for most of my work followed by a 3/8 CS to trim 0.2mm- 3mm excess horizontal material and 2mm vertical. It saves me a ton of tool life but does add a little to the machining time of course. I have to use a counterclockwise cut with the cleanup to get a perfect edge with the compression spiral but either works fine on the rough pass. I just try and keep the passes light so I can increase the depth of each cut as the main cutting area dulls. That makes better use of the overall cutting area.

Quote:

---

Originally Posted by Jake4

Hey Guys,

First-time poster, but hopefully can generate some good quality information from this.

Soo my this is where I am at.

I purchased a Biesse Rover J Plast a little over 4 months ago. I had a purchase order of 5,000 units of a product I designed. 5,000 units equaled to 25,000 finished CNC cut parts. 10,000 of those parts were from 9mm Hydrotek Marine Plywood and the remaining 15,000 units were out of 6mm Hytroket Marine Plywood. My shop is at around 6,000' of elevation I'm running 2) 25HP Becker Pumps paired with a 10HP (24000RPM HSD Spindle). My first issue arose with finding the correct spoil board. After many and many attempts, I settled with Ultra Light 1" MDF. This seemed to give the best hold-down and lasts until I get to about 1/2" thickness. PVC Edge banding.

Secondly was getting my feeds and speeds correct. I ended up purchasing GWiazrd and used their calculations. Needless to say, I burnt up my spindle in roughly a month and a half. Biesse said I was crazy for running my spindle close to maxed out, but the salesman said it will do 24k all day and night. Either way, the spindle was replaced by warranty. I'm reluctant to spin this above 22k now, but I suffered in completing this PO of 5,000 units, but it's finished. Now I have a PO of 20,000 units!

I'm back to testing and figuring out the best machining methods. I've purchased a second CNC to cut my 1,100 man-hours of routing in half. I'm not purchasing another Biesse. I was promised that it would not have any limitations, but only benefits from their processor. That is most assuredly not true on their 3 axis routers. It was complete and utterly a pain creating a post for fusion360 for this controller. If I did purchase another Biesse my post wouldn't work either so it's completely out of the question. Long story short I'm getting a machine that reads standard G-code with the same hardware specs.

Now back to testing, I'm finding that with my nested parts which range from 54-88 units per 4x8 sheet that I'm burning up bits in 2-3 sheets. I run as little as 7 sheets a day. In comparison to a cabinet shop, I'm doing enough cutting in a couple of hours than most see in a week. I've tried multiple different methods from slower to faster/ multiple depths/ doing a larger diameter to a smaller diameter in multiple passes/ all seem to dull bits at about the same amount of time. If the bit gets dull then my employees are sanding for the next month and it's moving my parts. So, in short, keeping my bits sharp seems to keep the operation as smooth as possible.

I've been using
Armana
46398-K 1/8 mortise compression
46200-K 1/8 down cut
46029-K 1/4 mortise compression
46181-K 3/16 mortise compression

Vortex
3115 mortise compression

These are my most recent test bits. I've used almost every other Armana bit out there that matches my type of cutting with the same results.

Sharpening bits seems to be out of the question because after my 2-3 sheets the hook on the end of the flute is basically sheared off. I have recently heard that all bits are meant to last for 15min of solid cutting. I do this in less than 20 min of my workday.

2 of my parts require hidden pocketing as which I need a router for. These 2 parts are the most time consuming and adds up to about 800 man-hours. The remaining parts are smaller and just need to be a 2d through-cut. I may switch to a laser cutter for these parts to eliminate the bit issue, moving part issue, headache, and be able to cut these parts in line with the router for reduced timing
.
As I said I am new to matching. I've been at it for 4 months and have overcome many hard-learned lessons, but I am still learning each and every day. I feel I have exhausted every contact I know. Most of my contacts that machine are primarily geared towards metal so their input has helped, but I've surpassed what they have been able to offer and now I'm strictly into the testing of high volume production with wood materials with machining methods.

The reason for this post is to generate any helpful knowledge I can pull from this user forum. Please don't hold back and give it to me straight.

Best,
Jake

---

How can I contact you?

CNC Cookbook has a great chipload calculator. I realized that I was running the cutters far slower than I needed. After years of burning through cutters in about a week, we not change them monthly and run nonstop all week long, 10 hours a day.