MechMate CNC Router Forum

Go Back   MechMate CNC Router Forum > After Building the Beast - Operating , Troubleshooting and Maintenance > General - MM Operating
Register Options Profile Last 1 | 3 | 7 Days Search Today's Posts Mark Forums Read

Reply
 
Thread Tools
  #1  
Old Wed 21 November 2007, 15:24
Richards
Just call me: Mike
 
South Jordan, UT
United States of America
Starting out to actually cut something - cutters, speeds, depths, directions, etc.

Sliced out of Charlie Trouse's thread . . .

Just yesterday, I managed to make the gantry on my Shopbot 60X120 jump the rails when I tried to cut MDF at full depth in one pass with a two flute 3/8-inch downcut spiral, spinning at 14,000 RPM and a feed speed of 7-ips with a 3-hp spindle. I've used that same configuration many times without trouble, but this time, I probably had a dull cutter in the spindle. I'd already cut 14 sheets of MDF with that cutter, and this time it just couldn't do the job. So, after putting the gantry back on the rails and re-zeroing everything, I adjusted the cut file to make two passes. That allowed me to cut three more sheets to finish the job without further problems. What I'm trying to say is that I'm not setup for high speed, full-out production. My machine, my spindle, my cutters and my vacuum system prefer multiple cuts rather than single cuts.
Reply With Quote
  #2  
Old Wed 21 November 2007, 23:29
Gerald D
Just call me: Gerald (retired)
 
Cape Town
South Africa
A good post Mike - thanks for taking it all the way to the reality of blunt cutters.
Reply With Quote
  #3  
Old Thu 22 November 2007, 10:23
Doug_Ford
Just call me: Doug #3
 
Conway (Arkansas)
United States of America
Yeah. Thanks Mike. My eyes always light up when I see you've posted a new message. I especially like your long posts because they are chocked full of useful and fascinating information.

With several years of experience under your belts, you and Gerald probably don't remember what it was like right before you received your first Shopbots. Since you didn't have to build them, you probably wondered about all the details involved in operating them. What's the best router bit? One pass or several? When will I know to change the spoilboard. How do I attach the spoilboard? Etc. When I first found this site, I wanted to see as many pictures of other machines as possible because I had to build mine. Since I finished the mechanical stuff, I'm now concerned with operating it and I'm probably where y'all were in the few weeks leading up to the delivery of your machines.

I've watched CNC mills operate in the past but never a CNC router. The operating details probably bore y'all now but your last paragraph contained exactly the kind of stuff I'd like to hear more about and I bet there are other guys that would agree with me. I would imagine that y'all might respond by saying, "Well, just ask and we'll tell you what you want to know." Unfortunately, I'm not sure what to ask. I guess what I'm saying is that I'd love to read a post from you in which you just talk about what you've discovered while operating your router. For example, in one post you said that you had conducted torture tests on motors in the past so I'm betting you've taken the same kind of scientific approach to testing router bits and feed speeds and probably other stuff too. Gerald has already determined the ideal motor so more detail on your motor tests is probably not appropriate but the other stuff would keep me enthralled for hours and would probably be useful to the other members of this forum. That is, if Gerald doesn't mind posts of that nature.

Thanks again.
Reply With Quote
  #4  
Old Thu 22 November 2007, 10:45
sailfl
Just call me: Nils #12
 
Winter Park, FL
United States of America
Yes, I would like to hear the experience of CNC users about what bit manufactures they found were the best. It is easy to go to a website and read what they have but experience is every thing.

Thanks
Reply With Quote
  #5  
Old Thu 22 November 2007, 11:24
Gerald D
Just call me: Gerald (retired)
 
Cape Town
South Africa
The first few days were spent pushing a pencil around - we were too scared to switch the router on!

Off the cuff: . . . .

Depth of pass between 1 and 2 bit diameters. (hardwood:1, softwood:2)

Bits. Solid carbide (not brazed/welded and definitely not "carbon steel"). The metalworker's milling cutters (2-flute, solid carbide) do a good job on wood and are generally cheap.

Best bits for starting out? Small cheap ones. . . . you are probably going to break them by cutting into a clamp or screw. Get bits that can plunge straight down (most small ones can)

Attach the spoilboard? The drawings should be telling you how?? (Glue only - no screws. Better go and check the drawings . . . . )
Reply With Quote
  #6  
Old Thu 22 November 2007, 11:34
Richards
Just call me: Mike
 
South Jordan, UT
United States of America
I'm a firm believer in testing. What works on one machine may not work on another. The first thing that I always do is to use a chipload calculator to determine the proper feed speed. Onsrud publishes a lot of useful information on their web site, including chipload formulas.

You can find that information here: www.onsrud.com/xdoc/ChipSoftwood

With a chipload of 0.015 inches, and a router/spindle RPM of 13,000 and a 2-flute cutter, the feed speed is: 0.015 X 13,000 X 2 = 390 inches per minute or 6.5 inches per second. That particular chip load works well for me with particle board, MDF and Baltic Birch plywood. Sometimes I go as high as 0.025, but I rarely go finer. You'll probably note that a router/spindle speed of 13,000 RPM is pretty slow for most routers. Before I installed a spindle, my Porter-Cable 7518 router didn't have much torque at 13,000 RPM. It preferred to run at 16,000 or 19,000 RPM. At those higher RPMs, the feed speed would have to increase to 8-ips or 9.5-ips to get the same chipload. Those higher feed speeds might be beyond the ability of most steppers (at least at a usable torque level). The way around that is to use a 1-flute cutter. That cuts the feed speed in half, which gives us more practical numbers.

Once the feed speed, RPM and cutter have been selected, I run a number of cuts in scrap material. Starting with a cut at least 12-inches long (so that ramping is not a factor), I make several cuts starting at 1/8-inch depth and progressing deeper in increments of 1/8-inch. While I make those cuts, I listen to the router and to the cutter. What I'm listening for is the sound of paper tearing. I've found that when everything is working properly, the cut sounds just like paper tearing. Also, if the router bogs down, I'm cutting too deep. After running the test, I know how deep I can cut without bogging down the router/spindle. I know the best RPM and feed speed to give me the quality of cut that I need, and I know that by using the recommended chip load, that I'll be getting the longest life out of the cutter.

With a spindle, I can easily increase or decrease the RPM as a cut is being made. With my particular spindle, 12,000 to 18,000 RPM gives full power, so I stay within those RPMs. When I was using the Porter-Cable, I almost always used either 16,000 RPM or 19,000 RPM in order to get adequate torque without burning up the cutter.

One other thing that you'll need to remember if you're cutting 3D or parts with lots of small moves is that ramping can really slow down the feed rate. On my Shopbot, small moves run at about 2-ips regardless of the speed that I've selected. So, I select an RPM and a cutter that gives me the proper chipload while running at a feed rate of 2-ips.

Anyway, that's the method that I use to determine the basic settings. Experimenting with different cutters, different feed rates and different router/spindle RPMs is part of the fun of owning a CNC router. I was surprised at the different settings that I had to use with different brands of cutters before the cut sounded right. For instance, a CMT cutter screams loudly at the settings that I use for an Amana or Freud cutter. In fact, I've found that CMT cutters are really picky when it comes to RPM. They cut very well, but having a spindle allows me to tweak things until the cut sounds right. Overall, now that I'm using a spindle, I'm getting at least 2X more life out of cutters than I got when I was using a router. I think that the difference is that the spindle holds its speed at a consistant RPM.

Edited: The chipload formula seems to work best when using moderate sized cutters. I almost always use either a 3/8-inch diameter cutter or a 1/4-inch diameter cutter. The chipload formula works well for those sizes; however, I always run extra tests with smaller cutters and cutters larger than 1/2-inch.

Last edited by Richards; Thu 22 November 2007 at 11:40..
Reply With Quote
  #7  
Old Thu 22 November 2007, 12:48
sailfl
Just call me: Nils #12
 
Winter Park, FL
United States of America
Mike,

Thanks for that useful information. It is a starting point for a new guy.
Reply With Quote
  #8  
Old Thu 22 November 2007, 22:13
Doug_Ford
Just call me: Doug #3
 
Conway (Arkansas)
United States of America
Thanks Gerald and Mike. I have a very slow and methodical approach to almost everything I do and I usually rehearse several times, in my mind, every step of an operation before I actually do it. The information y'all posted will give me lots to think about.

I finished making my router mounting brackets yesterday. I'm pretty happy with how they turned out. I'll try to get some pictures posted this weekend and another picture of my control box from the top for Abdul.
Reply With Quote
  #9  
Old Thu 22 November 2007, 23:01
Gerald D
Just call me: Gerald (retired)
 
Cape Town
South Africa
Doug, if you want a subject to ponder on, think about your direction of cut - ie. if you cut square cheesboards out of pine, do you go clockwise or anti-clockwise around them? There is a huge difference, and even a factor of direction for first pass versus second pass. Before "disclosing" the generally used method, I think it will be useful for you to chew on what happens where the bit meets the wood . . . . . .

How would that pine splinter on the corners? . . . .

Which way does the cutter (and MM) flex as it takes the cutting load? . . . . . .

Will the flex cause the cheeseboard to end up a little big, or a little small? . . . . .
Reply With Quote
  #10  
Old Fri 23 November 2007, 07:39
Doug_Ford
Just call me: Doug #3
 
Conway (Arkansas)
United States of America
Heh heh. I love puzzles like this but now I'm not going to get anything else done until I figure out the answer. Good thing I don't have to go to work today because I would be a menace during the morning commute, totally pre-occupied, putting along at 45 mph in the fast lane.
Reply With Quote
  #11  
Old Sun 25 November 2007, 16:39
Doug_Ford
Just call me: Doug #3
 
Conway (Arkansas)
United States of America
Gerald,

If you are making several passes, I would guess that as you approach each corner for the second time (and possibly the fourth corner for the first time), you will have a problem with the pine splintering on corners where you transition from cutting across end grain to cutting with the grain. So two out of the four corners will have a problem on one side of them. However, I have no idea what you can do about it except cut in from each corner to about halfway but that would waste alot of time. Is there an easier solution?

I'm guessing that the cutter and the MM will flex away from the boards until all of the slack in the machine is taken up. That will result in the part being slightly larger than desired.

When machining metal, I believe that a climbing cut normally produces a better surface finish than a conventional cut. But if your vertical mill has loose tolerances (like mine) a climbing cut can be dangerous because the cutting tool has a tendency to grab the work piece. For readers who don't know, a climbing cut is when the workpiece is fed with the direction the cutter is spinning and a conventional cut is when the workpiece is fed against the direction the cutter is spinning. I have no idea whether a climbing cut or a conventional cut is better when cutting wood. What's the answer?
Reply With Quote
  #12  
Old Sun 25 November 2007, 23:45
Gerald D
Just call me: Gerald (retired)
 
Cape Town
South Africa
Doug, food for further thought . . . . .

When you go anti-clock around the board (conventional), there is no splintering. Why not?

If you take a handheld router, with a bit spinning clockwise (viewed from top), and you are just starting to push a freehand dado groove away from you, the router kicks to the left........the spinning bit wants to roll along the edge of the board before it bites. When it does bite, it kicks viciously to the left. Go anti-clock around the cheeseboard (conventional) it is undersize, climb cut and it is oversize . . . . .

Very common to do 2 passes to get through a board. Two identical passes leave a mark in the middle. Two ways to be rid of the mark:
- first cut slightly bigger "toolpath" (more offset). Second pass on size and the upper part of the bit cleans the first pass. or
- first pass climb cut, second pass conventional - has same effect as above.

This "kick" to the left. . . . . Imagine cutting out a round pizza platter. Exact size not critical so you apply lots of force and speed. But, when the cutter has gone right around, and meets the starting point again, there is nothing to kick against. . . . all the flex relaxes. . . . and leaves a tiny mark on the job. Actually the same when the first cut starts after the plunge. The plunge is exact in its location, but as soon as the x,y movement starts there is a small flex.

Very few people will notice this flexing/kicking behaviour......unless the z-slide roller eccentrics are too loose, or they have long z-slides taking heavy cuts.
Reply With Quote
  #13  
Old Mon 26 November 2007, 08:39
Doug_Ford
Just call me: Doug #3
 
Conway (Arkansas)
United States of America
Gerald,

I hope you have the answers to these latest questions. If not, you are going to make me go insane. I'll ponder some more on these new questions. Thanks. I think.

Last edited by Doug_Ford; Mon 26 November 2007 at 08:42..
Reply With Quote
  #14  
Old Mon 26 November 2007, 09:02
Gerald D
Just call me: Gerald (retired)
 
Cape Town
South Africa
Doug, there is only one new question, about the splintering in one direction only. The rest of that post was supposed to be the answers!

Anyway, I will dig out, or make new, sketches on the splintering issue.
Reply With Quote
  #15  
Old Mon 26 November 2007, 10:43
Gerald D
Just call me: Gerald (retired)
 
Cape Town
South Africa
Here is a piece of white pine, the toolpath is blue:

Clipboard01.gif
Cutting A to B in the solid wood actually goes past the white corner at B and it cannot splinter because there is still solid wood behind the corner.


Clipboard02.gif
Going from B to C, the bottom of the cutter is going with the grain.


Clipboard03.gif
Changing direction at C is no problem because the cutter tip pushes the corner down (towards D)


If this job had started at D, corner D will splinter as the tool approaches it, because there will be no solid wood to support it:
Clipboard05.gif


Morals of the story:
1. Cutting into solid pine can minimise splintering - a "cleanup pass" can do more harm than good.

2. The starting/finish points need to be carefully selected.

3. Direction is very important.
Reply With Quote
  #16  
Old Mon 26 November 2007, 11:07
Doug_Ford
Just call me: Doug #3
 
Conway (Arkansas)
United States of America
Sorry Gerald. I realized that after I wrote it and I actually edited it twice but for some reason, the changes didn't take effect. Fascinating stuff. Thanks.
Reply With Quote
  #17  
Old Mon 26 November 2007, 13:37
Alan_c
Just call me: Alan (#11)
 
Grabouw (Western Cape)
South Africa
Send a message via Skype™ to Alan_c
Guys

Consider this (from personal experience of cutting waay too many toilet seats than is healthy) What gerald says above is correct if you are only cutting squares out of a solid board, and are only concerned with breakout on the corners but if one compares the cross grain cut finish of conventional versus climb cut, you will probably find that the climb cut will give you a better finish.

On something like a toilet seat or pizza platter the grain direction is consantly changing. With a conventional cut, it tends to tear out the end grain as it cuts across the grain as the wood fibres have no support but with a climb cut, the cutter is progressing into the timber which backs up the fibres being cut allowing the cutter to cleanly cut the fibres, this is much less of a problem with hard woods of course.

If I were doing a profiled edge on the workpiece, I would rough out the part using a conventional cut (can also handle bigger "bites"), change tools and do the profile cut using a climb cut. The rough cut would leave at least 3mm to be cut by the profiler. This usually gives me superior results.

Note I said "usually" above, there will be times with tricky cuts or difficult grain where I would take half of the cut in one direction, lift out got to the other end and cut in the other way and hopefully meeting nicely in the middle. As most of my work is long production runs, I can tweak the program to make sure my meeting point is accurate.
Reply With Quote
  #18  
Old Sat 12 January 2008, 11:53
Doug_Ford
Just call me: Doug #3
 
Conway (Arkansas)
United States of America
Gerald and Mike Richards,

When it comes time to resurface your spoil board, what do you use? Just a regular end mill or do you have a larger end mill with carbide inserts that will surface a 4 inch wide swath?
Reply With Quote
  #19  
Old Sat 12 January 2008, 12:31
Gerald D
Just call me: Gerald (retired)
 
Cape Town
South Africa
We use a 25mm [1"] diameter, carbide tipped 2-flute cutter sold for handheld woodwork routers (for making 1" dados?). It's a cheap cutter. Realise that this cutter cannot plunge vertically down.

The "pros" use bigger "planing" cutters, especially if they have the power and speed control of a spindle available to them. Middle of this page is an example.

Even with the relatively small 25mm [1"] cutter, re-surfacing the table takes less than an hour of un-supervised time.

Watch out for large diameter cutters - their max speed (before they "explode") can be quite low. (There are some big cutters sold as slower drill-press planers - don't put these in routers/spindles)
Reply With Quote
  #20  
Old Sun 13 January 2008, 06:45
Richards
Just call me: Mike
 
South Jordan, UT
United States of America
I use a Freud brand 1-1/2 inch diameter 2-flute bit. As Gerald mentioned, it was not designed to plunge into the material, so I have my surfacing program written to start off the spoil board, plunge to -0.075 inch and then cut.
Reply With Quote
  #21  
Old Sun 13 January 2008, 07:03
bleeth
Just call me: Dave
 
Florida
United States of America
I have been using a 1 1/4" mortising bit from Whiteside for years. (not the same one-It does need replacing occaisonally) I have found it to be a reasonably priced excellent bit for the purpose. The diameter is large enough to show if there are any Z misalignments and it handles all the depth and more than I have ever needed.
Reply With Quote
  #22  
Old Sun 13 January 2008, 07:28
Gerald D
Just call me: Gerald (retired)
 
Cape Town
South Africa
Quote:
Originally Posted by Richards View Post
I use a Freud brand 1-1/2 inch diameter 2-flute bit. As Gerald mentioned, it was not designed to plunge into the material, so I have my surfacing program written to start off the spoil board, plunge to -0.075 inch and then cut.
Imagine using a 4" diam. cutter . . . . . . . then the router must start 2" off the table. I did add 50mm [2"] to the design all round, so this would be right on the limits of the machine's capability.
Reply With Quote
  #23  
Old Tue 09 July 2013, 04:02
silverdog
Just call me: Sergio #70
 
Rome
Italy
Onsrud Guide

Don't know if already posted ... I found it very interessing.
Sergio
Attached Files
File Type: pdf onsrud_routing_guide.pdf (938.2 KB, 89 views)
Reply With Quote
Reply

Register Options Profile Last 1 | 3 | 7 Days Search Today's Posts Mark Forums Read

Thread Tools

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off

Forum Jump


All times are GMT -6. The time now is 14:28.


Powered by vBulletin® Version 3.8.3
Copyright ©2000 - 2017, Jelsoft Enterprises Ltd.