This Is So Mechanical...

[Prostheta]

I suppose if you can't work out the specifics you should listen to the router complain, right?

[RestorationAD]

Difficult to see from the photos but it looks like you are producing more dust than chips. How do you calculate your speed/feed/chipload/etc?

Funny enough the pine is producing a combination of long strips that peel off like when machining aluminum and nice 1/16" sized chips. No real dust at all. I will get a better idea of chip clearance when I start testing in harder woods... I think Lowe's 2x8s are really a bad test medium as they are not dry enough.

I've no direct experience (yet, soon!), but I used to see very similar problems with my first router, which could only take small bits. More power and larger bits that don't flex allow the cutting edges to just do their work without introducing additional friction; the finish you get with a 2.5HP router and a 1/2" bit is significantly better than what you can achieve with the same router and a 1/4" straight bit. Upgrading one or both will certainly help quality of cut. It's easier to adjust when you're working handheld, because you can 'feel' when the bit's getting bogged down and back off a little. The CNC can't.

Good point. But I am not upgrading the spindle for a while.

I suppose if you can't work out the specifics you should listen to the router complain, right?

Yeah you can hear it when you push it too hard. Using just the ear test I can probably get close.

[Prostheta]

Still at that scary unanticipated point where you really need to get chunking into the real wood, but feel you need to keep testing the waters first?

I think I remember feeling that the first time I decided to try routing Perspex. No real way of getting the feel for it until you get in and commit. Scary.

[RestorationAD]

Still at that scary unanticipated point where you really need to get chunking into the real wood, but feel you need to keep testing the waters first?

I think I remember feeling that the first time I decided to try routing Perspex. No real way of getting the feel for it until you get in and commit. Scary.

Yes. I foresee a few expensive mistakes in my future.

[pauliemc]

ducati?

Amazing machines. I have a 748R, goes like fresh cow **** off a greased shovel

But im selling it to raise the rest of the cash for a CNC.

Gona suck lettin it go

But thats ok. I still have my tweaked Harley for runnin around on

[RestorationAD]

ducati?

Amazing machines. I have a 748R, goes like fresh cow **** off a greased shovel

But im selling it to raise the rest of the cash for a CNC.

Gona suck lettin it go

But thats ok. I still have my tweaked Harley for runnin around on

Last few bikes...

1995 900ss CR (My favorite)

2005 BMW 1100s Boxer Cup

2006 749s

2007 S2R Monster

I sold my 749s because 140 felt like cruizing speed and my kid needs her dad (I have custody). The S2R Monster is a consolation prize. It and I are not the friends I wanted to be (me and the 749s were tight)

however....

No way I would let it go to build guitars with a Computer.

I think your passion for building is awesome.

[MiKro]

Ok Rad, I have a few questions for you. What is your max feed rate without load or any step loss/midband resonance problems? Also what Controller software are you using? What is your max End mill shank diameter ( I'm guessing 1/4"), and what is your spindle speed variance and how is it achieved? meaning what is the speed control for the router. Also what type of end mills or router bits are you using? Once I have some of this I may be able to guide you better . What brand of Router/spindle as well

Mike

[RestorationAD]

Ok Rad, I have a few questions for you. What is your max feed rate without load or any step loss/midband resonance problems? Also what Controller software are you using? What is your max End mill shank diameter ( I'm guessing 1/4"), and what is your spindle speed variance and how is it achieved? meaning what is the speed control for the router. Also what type of end mills or router bits are you using? Once I have some of this I may be able to guide you better . What brand of Router/spindle as well

Mike

Max feedrate is probably 100 IPM (never been above 45)

Controller Software EMC2

Max End Mill .250 (for now)

Spindle Speed Variance 16,000 to 35,000 rpm (I have a dial on the top of the router so set and forget)

End Mill 2-flute .25 End Mill 1.25" flute length 4" overall (chinese cheapo for now)

Spindle Bosch Colt Palm ( regret not getting a better spindle right at the momment. Will upgrade before end of year)

[pauliemc]

No way I would let it go to build guitars with a Computer.

I think your passion for building is awesome.

Guitars are what I do, Bikes are next in the line of "Must haves". So long as my Klunker (tweaked harley) is here with me then the bike part is sorted.

I need some cash & some room for a CNC so the 748R is going. Someone else can enjoy the banana bullet for a while (its yellow, hence the bananna bit)

It kinda sucks letting it go, but I got an order a few weeks ago for 40 gitirs from a customer & its killing me getting it done. So if the machine can sort most of the roughing out, neck pockets, truss slots etc then I can get things done without 75-80 hour weeks becoming the norm, which they are just now.

[RestorationAD]

No way I would let it go to build guitars with a Computer.

I think your passion for building is awesome.

Guitars are what I do, Bikes are next in the line of "Must haves". So long as my Klunker (tweaked harley) is here with me then the bike part is sorted.

I need some cash & some room for a CNC so the 748R is going. Someone else can enjoy the banana bullet for a while (its yellow, hence the bananna bit)

It kinda sucks letting it go, but I got an order a few weeks ago for 40 gitirs from a customer & its killing me getting it done. So if the machine can sort most of the roughing out, neck pockets, truss slots etc then I can get things done without 75-80 hour weeks becoming the norm, which they are just now.

Good enough as long as you still have one bike.

Don't think the CNC is going to help right away. I am learning that it has a learning curve... then again if I was serious I could speed up the learning curve.

[MiKro]

Ok Rad, I have a few questions for you. What is your max feed rate without load or any step loss/midband resonance problems? Also what Controller software are you using? What is your max End mill shank diameter ( I'm guessing 1/4"), and what is your spindle speed variance and how is it achieved? meaning what is the speed control for the router. Also what type of end mills or router bits are you using? Once I have some of this I may be able to guide you better . What brand of Router/spindle as well

Mike

Max feedrate is probably 100 IPM (never been above 45)Okay then first you need to setup at maximun Feedrate for Maple or about any wood. you will need to set your pass depths at approx 30% +/- 5%. stepover no more than 26%.These are not set in stone but places to start, yo may have to reduce your feed rate by 10% or maybe the DOC. Alos learn to edit your GCode, Slow the feedrate on the first full width cut to 40-50IPM then speed up for the stepover passes.

Controller Software EMC2 (not my choice, PM me about M3 there is a free version that does not have limits)

Max End Mill .250 (for now) Okay then buy some true end mills for cutting metal.

Shars.com

Long length

Spindle Speed Variance 16,000 to 35,000 rpm (I have a dial on the top of the router so set and forget) Set for about 18K-20K rpm, I veryrarely go above 14K but I believe you will lose to much torque

End Mill 2-flute .25 End Mill 1.25" flute length 4" overall (chinese cheapo for now) See above Also try a 4 flute in short as well.

Spindle Bosch Colt Palm ( regret not getting a better spindle right at the momment. Will upgrade before end of year) Go with a Porter cable easier to get parts for need only a 690R no bigger. Get precision collets for it. 1/8",1/4"/ 1/2" also if you upgrade to Mach3 add a Super PID 2 Speed control, allows for computer control of router and no degradation of torque at lower RPMs, will go down to 5000 rpm.

With the above, try some test cuts ad see what happens.

Mike

[RestorationAD]

Max feedrate is probably 100 IPM (never been above 45)Okay then first you need to setup at maximun Feedrate for Maple or about any wood. you will need to set your pass depths at approx 30% +/- 5%. stepover no more than 26%.These are not set in stone but places to start, yo may have to reduce your feed rate by 10% or maybe the DOC. Alos learn to edit your GCode, Slow the feedrate on the first full width cut to 40-50IPM then speed up for the stepover passes.

Ok this makes sense I was thinking about this the other day.

Controller Software EMC2 (not my choice, PM me about M3 there is a free version that does not have limits)

Ok.

I am using EMC2 and linux machine to power it. I like it so far because I know Linux and it seems like a really good solution... However I have never used anything else.

What am I going to gain by switching to M3?

Max End Mill .250 (for now) Okay then buy some true end mills for cutting metal.

Shars.com

Long length

End Mill 2-flute .25 End Mill 1.25" flute length 4" overall (chinese cheapo for now) See above Also try a 4 flute in short as well.

Already on the way.

Spindle Speed Variance 16,000 to 35,000 rpm (I have a dial on the top of the router so set and forget) Set for about 18K-20K rpm, I veryrarely go above 14K but I believe you will lose to much torque

Ok.

Spindle Bosch Colt Palm ( regret not getting a better spindle right at the momment. Will upgrade before end of year) Go with a Porter cable easier to get parts for need only a 690R no bigger. Get precision collets for it. 1/8",1/4"/ 1/2" also if you upgrade to Mach3 add a Super PID 2 Speed control, allows for computer control of router and no degradation of torque at lower RPMs, will go down to 5000 rpm.

Not going to be able to do this until later in the year as it is a bigger investment. But I will. I have to decide in November whether to upgrade this machine or sell it and buy a bigger machine. No point in buying a bigger Router Spindle when I might buy a bigger machine with a true spindle at the end of the year.

[MiKro]

So here is a test pocket Gcode of a 2" by 1" square raster pocket with a 1/4" EM, Feed rate 185 IPM and DOC per pass at 0.075 and stepover of .1

X and Y zero at center. Z0 at top

See the red highlights and notes. You will need to do this at all of the places of DOC change to maximize your speed and not burn wood or load the spindle. This will work until you can upgrade to a larger router. All it takes is understanding what the code is doing and where. All the editing is done in Notepad..

( Testpocket )

( File created: Friday, March 16, 2012 - 01:25 PM)

( Mach2/3 Arcs Inch )

( Material Size)

( X= 4.000, Y= 4.000, Z= 1.500)

()

(Toolpaths used in this file:)

(Pocket 1)

(Tools used in this file: )

(1 = End Mill {0.25 inch})

N100G00G20G50G17G90G40G49G80

N110G70G91.1

N120T1M06

N130 (End Mill {0.25 inch})

N140G00G43Z1.0000H1

N150S15000M03

N160(Toolpath:- Pocket 1)

N170()

N180G00G94G4P07

N190X0.0000Y0.0000F185.0

N200G00X0.8600Y-0.3414Z0.5000

N210G00Z0.2500

N220G1Z-0.0833F15.0

N230G1X-0.8600F185.0This is the first pass, change feed rate, it needs to be changed to 50% of max.

N230G1X-0.8600 F90.0This is the new value

N240G1Y-0.2664 Note this is the first stepover

N250G1X0.8600 F185Note now I up the feed rate by adding the F185 to the line

N260G1Y-0.1914

N270G1X-0.8600

N280G1Y-0.1164

N290G1X0.8600

N300G1Y-0.0414

N310G1X-0.8600

N320G1Y0.0336

N330G1X0.8600

N340G1Y0.1086

N350G1X-0.8600

N360G1Y0.1836

N370G1X0.8600

N380G1Y0.2586

N390G1X-0.8600

N400G1Y0.3336

N410G1X0.8600

N420G00Z0.5000 This move is a move to the final pass before DOC change, The reason for the change in Z. It's going to a rapid, to start the final pass Note the G0 command not G1.The G1 commands highlighted are the final pass. Then a G0 rapid before the next DOC

N430G00X-0.8750Y0.3750

N440G00Z0.2500

N450G1Z-0.0833F15.0

N460G1X0.8750F185.0

N470G1Y-0.3750

N480G1X-0.8750

N490G1Y0.3750

N500G00Z0.5000

N510G00X0.8600Y-0.3414

N520G00Z0.2500

N530G1Z-0.1667F15.0Note here we have the start of the next DOC

N540G1X-0.8600F185.0here we make the change to slow down again, Change to F90

N550G1Y-0.2664

N560G1X0.8600here we make the change to higher feedrate again, add F185

N570G1Y-0.1914

N580G1X-0.8600

N590G1Y-0.1164

N600G1X0.8600

N610G1Y-0.0414

N620G1X-0.8600

N630G1Y0.0336

N640G1X0.8600

N650G1Y0.1086

N660G1X-0.8600

N670G1Y0.1836

N680G1X0.8600

N690G1Y0.2586

N700G1X-0.8600

N710G1Y0.3336

N720G1X0.8600

N730G00Z0.5000

N740G00X-0.8750Y0.3750

N750G00Z0.2500

N760G1Z-0.1667F15.0

N770G1X0.8750F185.0

N780G1Y-0.3750

N790G1X-0.8750

N800G1Y0.3750

N810G00Z0.5000

N820G00X0.8600Y-0.3414

N830G00Z0.2500

N840G1Z-0.2500F15.0

N850G1X-0.8600F185.0

N860G1Y-0.2664

N870G1X0.8600

N880G1Y-0.1914

N890G1X-0.8600

N900G1Y-0.1164

N910G1X0.8600

N920G1Y-0.0414

N930G1X-0.8600

N940G1Y0.0336

N950G1X0.8600

N960G1Y0.1086

N970G1X-0.8600

N980G1Y0.1836

N990G1X0.8600

N1000G1Y0.2586

N1010G1X-0.8600

N1020G1Y0.3336

N1030G1X0.8600

N1040G00Z0.5000

N1050G00X-0.8750Y0.3750

N1060G00Z0.2500

N1070G1Z-0.2500F15.0

N1080G1X0.8750F185.0

N1090G1Y-0.3750

N1100G1X-0.8750

N1110G1Y0.3750

N1120G00Z0.5000

N1130G00X0.8600Y-0.3414

N1140G00Z0.2500

N1150G1Z-0.3333F15.0

N1160G1X-0.8600F185.0

N1170G1Y-0.2664

N1180G1X0.8600

N1190G1Y-0.1914

N1200G1X-0.8600

N1210G1Y-0.1164

N1220G1X0.8600

N1230G1Y-0.0414

N1240G1X-0.8600

N1250G1Y0.0336

N1260G1X0.8600

N1270G1Y0.1086

N1280G1X-0.8600

N1290G1Y0.1836

N1300G1X0.8600

N1310G1Y0.2586

N1320G1X-0.8600

N1330G1Y0.3336

N1340G1X0.8600

N1350G00Z0.5000

N1360G00X-0.8750Y0.3750

N1370G00Z0.2500

N1380G1Z-0.3333F15.0

N1390G1X0.8750F185.0

N1400G1Y-0.3750

N1410G1X-0.8750

N1420G1Y0.3750

N1430G00Z0.5000

N1440G00X0.8600Y-0.3414

N1450G00Z0.2500

N1460G1Z-0.4167F15.0

N1470G1X-0.8600F185.0

N1480G1Y-0.2664

N1490G1X0.8600

N1500G1Y-0.1914

N1510G1X-0.8600

N1520G1Y-0.1164

N1530G1X0.8600

N1540G1Y-0.0414

N1550G1X-0.8600

N1560G1Y0.0336

N1570G1X0.8600

N1580G1Y0.1086

N1590G1X-0.8600

N1600G1Y0.1836

N1610G1X0.8600

N1620G1Y0.2586

N1630G1X-0.8600

N1640G1Y0.3336

N1650G1X0.8600

N1660G00Z0.5000

N1670G00X-0.8750Y0.3750

N1680G00Z0.2500

N1690G1Z-0.4167F15.0

N1700G1X0.8750F185.0

N1710G1Y-0.3750

N1720G1X-0.8750

N1730G1Y0.3750

N1740G00Z0.5000

N1750G00X0.8600Y-0.3414

N1760G00Z0.2500

N1770G1Z-0.5000F15.0

N1780G1X-0.8600F185.0

N1790G1Y-0.2664

N1800G1X0.8600

N1810G1Y-0.1914

N1820G1X-0.8600

N1830G1Y-0.1164

N1840G1X0.8600

N1850G1Y-0.0414

N1860G1X-0.8600

N1870G1Y0.0336

N1880G1X0.8600

N1890G1Y0.1086

N1900G1X-0.8600

N1910G1Y0.1836

N1920G1X0.8600

N1930G1Y0.2586

N1940G1X-0.8600

N1950G1Y0.3336

N1960G1X0.8600

N1970G00Z0.5000

N1980G00X-0.8750Y0.3750

N1990G00Z0.2500

N2000G1Z-0.5000F15.0

N2010G1X0.8750F185.0

N2020G1Y-0.3750

N2030G1X-0.8750

N2040G1Y0.3750

N2050G00Z0.5000

N2060G00Z1.0000

N2070M05M09

N2080G00X0.0000Y0.0000

N2090M30

%

[RestorationAD]

Mikro,

Excellent.

I won't be able to test until Saturday. I will let you know when I have it worked out.

[MiKro]

What am I going to gain by switching to M3?

Better support from people like me. There are other things, but at this time it is a moot point.

[RestorationAD]

Slowing the spindle helped immediately. I am working on editing the gcode for tomorrows runs.

[MiKro]

Slowing the spindle helped immediately. I am working on editing the gcode for tomorrows runs.

Very good. Stick with it. If need be, cut air for the Gcode test to make sure what is happening before cutting wood. When testing in the wood, the key will be finding the correct feedrate for the RPM to not overload your router and make small chips. Not Dust,if you are making dust then you will burn the wood. That's why I use metal endmills. They are for slower RPM's, They remove wood easily and last so much longer than a Router bit at 1/2 to 1/3rd the cost. Oh! and they are much sharper as well. YOU may want to do a final pass set as a climb cut,this will also make it cleaner. For a final pass, say on a PU cutout choose a profile toolpath, choose inside(make sure your vectors are joined also verify that the arrows on the screen are inside the vector) and change your passes DOC((edit this 0nly in the toolpath not the endmill tool database)) to max diameter and make the final passes with that after the pocket cuts are done. Since all of the material is already cut this is almost a no load cut to cleanup, use Climb for this. just save both toolpaths together in Asp3 (Click check for both of them when saving since they use the same Endmill). Just make sure it is the last in line.

MK

[RestorationAD]

Thank you Mikro for all the help.

SO I made nice chips all day Sunday. No dust. If I was able to cut _old_ black Ash well Mahogany should be a breeze.

It took a while to find the right DOC and feedrate for the slowest spindle speed but it worked.

Now I have to work on roughing vs finishing passes. I have a small chip tear-out on the bridge humbucker (almost identical to what you would get with a hand router) near the tab. So my plan is to rework all the code this week to rough within .020 then come in with 2 .010 climb cuts to clean up pockets. It takes a long time to cut the bodies right now but the important part is to get it right. I will worry about optimization in coming weeks.

My new carbide mills should be in this week which should help immensely.

[Prostheta]

Video is marked as private, RAD.

[RestorationAD]

Video is marked as private, RAD.

Fixed... YouTube FAIL .

And you would think I of all people would know how to work that stuff...

[MiKro]

Thank you Mikro for all the help.

SO I made nice chips all day Sunday. No dust. If I was able to cut _old_ black Ash well Mahogany should be a breeze.

It took a while to find the right DOC and feedrate for the slowest spindle speed but it worked.

Now I have to work on roughing vs finishing passes. I have a small chip tear-out on the bridge humbucker (almost identical to what you would get with a hand router) near the tab. So my plan is to rework all the code this week to rough within .020 then come in with 2 .010 climb cuts to clean up pockets. It takes a long time to cut the bodies right now but the important part is to get it right. I will worry about optimization in coming weeks.

My new carbide mills should be in this week which should help immensely.

Looking good.Just remember that you will use the offset function in ASP3 to make the roughing vs finish paths. Check your paths on screen to make sure you are going in the correct direction with the offset. So to exaggerate this (to visualize it)try + 0.100 and -0.100 to see which way you need, based on an inside or outside toolpath and climb or conventional. Then set for the actual offset you need.

That way your profile passes will not need to be duplicated in the drawing using offset vectors. Also when genning tool paths look at the Tab function if needed, It can make a difference in setup for flipping. I will try and explain it when you are ready to use it.

As far as pockets. Set your roughing passes at the 0.010 or 0.020 offset and then generate finish toolpath.

MK

[RestorationAD]

New carbide end mills made a huge difference...

Now I have a new issue. For some reason on the last body pickup routes the machine decided to bump when it hit the corners on the final clean up pass. This of course caused it to miss a step and start cutting out of wack full depth... needless to say it is a good thing I was standing there watching it.

Pickup pockets are hard because they are so small...

I am trying to find the best pathing option for routing cavities and so far a few of the things I have tried were bad ideas. I am not sure why on the final passes of 0.015 DOC and cleaning up a 0.005 roughing distance the bits are jumping. I have had a similar problem with spiral template router bits in the past. Maybe I need to do a better job sneaking up on the outer edge.

One thing I am considering is using a outline profile first then cleaning the pocket out with a 0.015 roughing distance so the bit doesn't touch the sides as it cleans out the pocket. The new bit cuts beautiful profiles so maybe that is the answer.

I will post some pictures and video tonight.

[HuntinDoug]

All good advice from Mike I'll give a hearty "Amen" to the Mach3 suggestion. I've never used anything else, so I'm a bit bias.

My question is: how much Z flex are you dealing with? These small entry level machines often have so much that it can be dangerous to climb cut.

[RestorationAD]

All good advice from Mike I'll give a hearty "Amen" to the Mach3 suggestion. I've never used anything else, so I'm a bit bias.

My question is: how much Z flex are you dealing with? These small entry level machines often have so much that it can be dangerous to climb cut.

I have a bit of Z-axis flex... it can actually deflect enough to see it visually if you push the machine to hard. I am trying to use the normal CNC methods to machining so I rough pass, then come back with a smaller step over/DOC and do a climb cut on the finish pass.

I wonder if I am getting a bit of backlash on the move in the corner and I can solve the issue with better pathing.

That would make sense as the final pass is always a climb cut. It was fine in Ash but the second blank was Mahogany and it seemed "grabby" if you know what I mean.

I cut 2 padauk neck blanks and the first I had terrible tear-out because of the grain orientation in relation to the regular pass. So I switched it over to a climb cut and had no more issues. However Padauk is a hard wood that is not as "grabby" per say.

I guess I need to develop a strategy for pocket cuts until next year when I upgrade the machine.

[MiKro]

All good advice from Mike I'll give a hearty "Amen" to the Mach3 suggestion. I've never used anything else, so I'm a bit bias.

My question is: how much Z flex are you dealing with? These small entry level machines often have so much that it can be dangerous to climb cut.

A good point Doug is making about the climb cut and flex.

question for you RAD. does EMC2 have a plasma function? If so, it will use an algorithm that will smooth out the passes. By not stopping at exact points. This is very handy when trying to maximize speed on curves and cuts out jerking of the machine. Now the problem when using this mode is that exact stop features are turned off and if you are trying to get exact 90 corners it will round them some. But most PU pockets have a radiused corner so this would help smooth that out.

If you look at your vectors in node edit mode you will see all of the points/nodes. The machine interprets these at point to point starts and stops at each one. The closer they are more jerking. Plasma mode will smooth that out. This is a function I use in Mach3 all of the time when doing 3d work and curved 2d work.