The results from testing today.

I am cutting the same grape file but this time I cut it in Oak and I added another bit.

Rough Cut - 1/4 End Mill - Onsrud 56-285. 22 Min / 125 IPM, 5 passes.

Relief Cut - 1/4 Ball Nose - Onsrud 52-280B. 20 Min / 125 IPM, 1 pass.

Relief Cut 2 - 1/8 Ball Nose - Onsrud 52-240B. 51 Min / 125 IPM, 1 pass.

I couldn't believe it took so long for the last cut. I am a little disappointed in that it did not clean up as well as I thought it would be that I suspect is because of Oak. Softer. The bits are new or with very little use.

I think I will cut this file again but in cabinet plywood and increase the speed. I would like to see how fast I can go. Plywood because it is a little softer and not as hard on the bits.

I had a little trouble getting the last bit at the right height so I will be working on completing my zero touch plate.

The first pic is after the rough cut and the last pic is after all three bits finished.

Hi Nil that start the year nicely ,good work. I reread your post and you say 2 1/4 hr per sf. and yes it seem long .What is your step over ? in roughing pass you can go 100%, for the finishing pass that is where you decide how much sanding versus machining you want to do. Your wood look like 3/4 thick? if so 3 maybe 2 stepdown passes should be enugh . Cranking up the speeds and wearing those earmuff will surely reduce time. Keep posting your progress
Normand

Nils for the relief cut 2 - think if you use a 30 degree V bit which is used for engraving then the finish in the leaf would be better - I have a art cam guru near my place who uses the V bit for the carvings

http://forum.artcam.com/viewtopic.ph...hlight=winfred

chk the video here -

RGDS
irfan

Yesterday, I did some more testing.

I cut the same file but I modified the feed speed from 125 to 200. All the other settings I left the same. I also only used two bits. I did not use the 1/8 ball nose.

The 1/4 end mill took 18 mins and the 1/4 ball nose took 18 mins but the quality of the cuts was noticeably different. For the small saving in time with the first two bits over the loss of quality of cut, I don't think speeding things up helps.

I would like to get a 30 deg V bit and see how that works.

I need some one with a little more experience to expain the advantage of increasing the router speed and the feed speed. Logically, it does not make sense to me that if I increase the speed of the router and the feed that the cut is going to get better. I used the router speed of 14000. It seems to me that you want the router speed to match the recommended speed of the bit. Then you need to find the best feed speed for the material you are cutting.

It would seem to me that the router speed is going to be the same for a specific bit you are using but that the feed speed is gong to change based on the material you are cutting with that bit.

One of the other things I found interesting is that with the higher speed, the rough cut did not do as good a job at the end of each X pass. It did not go the full X on each Y.

Nils what is your accelerations settings when you are roughing the part. are you able to set a little more accln - may be that should solve the problem.

RGDS
Irfan

When you are doing finishing with a 1/4" ball nose bit, it is maybe only the center 1/8" that is doing the work. So your spindle/router speed needs to be set for a 1/8" diam bit.

A popular source of cutters for the SB'ers:
http://www.beckwithdecor.com/index.htm

Nils,

Onsrud has great technical articles and information.

https://www.onsrud.com/

Gerald,

I have been doing some testing to understand if my machine is cutting correctly and to understand its capabilities.

These test are done with a 1/4 End Mill with the router set at its maximum RPM of 22,000. The accelration is set for X and Y at 10.

The first picture is 1" X cuts (up and down) moving 3/4" on the Y. For each X Y pair (Up and Across legs), the IPM was the same. The first leg was set at 150, 200, 250, 300, 350. The bottom pair was 1/4" Deep and the top was at 1/2" Deep. The cuts start in the lower Left Hand side.

The results are very good but the distance is not very far.

The second picture is 5" X cuts and moving 3/4" on the Y. Again for each X Y pair same setup. The first leg was set at 100, 150, 200, 250, 300, 350, 400, 450. The starting point is the same and the depth of the cut is 1/4" deep.

The cut results are starting to get bad at the end of the 200 X run.

The final cut should look like the first picture but with the X 5" long.

Am I expecting too much here or should my results be better and I need to make an adjustment?

Are there some better test parameters that I should be using?

You don't seem to be in "Exact path mode". In EMC GCode terms, you should have G61 or, or at least something like G64 P0.01
http://www.linuxcnc.org/docs/2.2/htm...1,-G61.1,-G64:

You'll want to find the right settings for your software.

Your X,Y accel settings should be a lot higher . . . 20 to 25.

Then, have a look at Kobus's thread, he saw something similar in the beginning.

Gerald and Brad,

Thanks for the input. I will do some more research on the GCodes and I will up my Acceleration.

Testing is a good thing.!

Nils,

Follow Brad and use the G61.

Yuri & Brad, I am not familiar with the G61 command in Mach. I think the equivalent is CV (constant velocity) mode versus "exact stop" done in a config setting . . .

I have retested and I am still having a problem.

I tested at a velocity of 20 and 25, with G61 and G64 Po.o1.

The best results that I am getting are with either 20 or 25 but with G61 added to the code. I am seeing a problem at the bottom of the cut but not at the top. The top cuts all have solid corners but the bottom you can see the extended. I am not sure how to describe it.

The first at 20 and the second at 25.

Same file for evey thing else.

What is causing this problem?

According to http://www.machsupport.com/docs/Mach3Mill_1.84.pdf on Page 63, exact stop mode is G61, constant velocity is G64. Pages 118/119 seem to imply that Mach does understand these values. Although G61 should be exact path, not exact stop (That's G61.1); this may be a documentation error.

Nils, I'd expect the following behavior from your machine:

Setting G61 or "exact path mode" should result in cutting that is correct, but noticeably slower.

Setting the accel/decel higher should both correct much of that slowness in G61 mode, and possibly make it reasonable to run in "constant velocity" or G64 mode.

You may want to explore if Mach3 supports the precision parameter of G64 (which is generally how I run my Mechmate). If it does, then:

G64 P0 should be essentially equivalent to exact path mode.
G64 P1 should constrain errors to within an inch (or mm, if you're in that mode).
G64 P0.125 should constrain errors to within an eighth inch.
G64 P0.01 should constrain errors to near undetectable.

Disclaimer: I've never run Mach3 nor seen it run. I believe that the text from the EMC manual is accurate to common G Code implementations, though:

We use a post processor for Artcam - EMC2(Linux).

Yuri, yes; G64 allows for errors, and just like riding a bike, more speed means more rounding.

Nils, you could post the GCode if you want, but I suspect you may have just left my comfortable world of software and moved to the cold hard world of mechanical tuning for that remaining error. Gerald, I think you're on now ...

Nils, that divot in the corner would make me grab the collet and shake everything to check for looseness. . . . your clockwise spinning cutter seems to be veering left as it takes cutting load.

Okay,

I will post the code.

Gerald, Please explain why I don't see the problem at both ends of X. I can not find that the collet is loose.



%
G90
G20
G49
G61
M3 S20000
G0 X0.000 Y0.000 Z0.573
G1 Z-0.250 F30
G1 X0.000 Y0.000 Z-0.250 F100
X5.000
Y-0.750
X0.000 F150
Y-1.500
X5.000 F200
Y-2.250
X0.000 F250
Y-3.000
X5.000 F300
Y-3.750
X0.000 F350
Y-4.500
X5.000 F400
Y-5.250
X0.000 F450
G0 Z0.573
G0 X0.000 Y0.000 Z0.573
G0Z0.573
X0.000Y0.000
M05
M02
%

At the bottom of the board, the cut path makes 2 left turns, at the top it makes 2 right turns.

One of the left turns is from X to Y while the other is from Y to X. Therefore, each of those 4 turns is unique.

If it is not looseness, then it could be plain flex - something bending to take load. How far is your cutting bit sticking out of the collet? (Keep that as short as possible or use a thicker bit)

The GCode is obviously fine.

I think Gerald was implying that you should check whether something mechanical anywhere on the machine is loose, from the perspective of the collet. You're tugging on the collet not to check just the collet, but everything. For example, does the Gantry run vertically relative to that photo, and has a little play developed in the X axis motor / gear at the bottom of the picture?

(Added text a few minutes later): Wait a sec, both the photo of your leg, and the GCode indicate that the overshoot is on the Y axis. So that would mean play on the Y Motor, the Y idler, or side-to-side on the Z plate / rollers.

Gerald,

You know your machine. I went back out and checkd for anything that might be loose. Yes, the Y car moved even with power.

My question is this. How tight do you make the Fixed A and Slotted B bolts for the motor plates. I loosened up Slotted B and the Y car didn't move.

Playing with the motors to retune and adjusting the springs, I might not have checked that things were set up right. Doesn't there need to be a little play in the Slotted B bolt even with the plastic washers?

Once I fixed the Y car, I ran the file again and the cut looks good in all directions.

I have also tested my Milwaukee router runout and it is not good. Mine is 0.003.

I have learned a good lesson. When the machine is not cutting right, first check to see if there is some thing loose!

Today, I made a part for my washer. It is a basic machine. I recently had to replace the waste water hose because a mouse ate through it. The washer is outside on my back porch. He must have taken the part I had to replace.

The part is in white in the picture. I milled it out of PVC board. I though I would need glue but it fits on tight. I am still learning so it took me a few tries to get it right but it works.

Zero Touch Plate

Today I changed the setting in Ports and Pins and got my Zero Touch Plate working. Beside the Shuttle Pro, Zero Touch Plate and the Laser make setting up the machine for a cut so easy.

My version is different than what I have seen others doing. I do not use any input on a Mach screen to monitor my Touch Plate. Yes, you will see the inputs on the Diagnoistic page but I use an LED. I use a button on the Shuttle Pro to activate the macro that drives the router to the touch plate.

I have an LED as part of the circuit. Before I run the macro, I touch the plate to the bit or router. If the LED turns Blue, that is the color I am using, I know that I will not drive the bit through the touch plate. Currently I have an alligator clip that attaches to the small wire that is above the LED in the picture. I will most likely use the red wire and replace the alligator clip and cut the black and other wire.

Nils,

Nice design. I love the LED idea.

Regards,
John

A good innovative streak you have there Nils! (including the "washer")

Our local language use:
washer: exclusively used under a screw head or nut
washing machine: for washing textiles - laundry equipment
dishwasher: kitchen equipment

John,

Thanks

Gerald,

I didn't really think it up as you know, I just made a slight modification that worked for me. I wanted some thing that would allow me to use the touch plate with out having to be at the computer to operate the touch plate macro. But reading the thread about a external switch and the touch plate has made me realize I have to have a way to stop the routine if I accidently hit the button on the shuttle pro during a job run. I will need to do some additional testing and experimenting.

My next project, since I don't have a lot of light in my garage, is to add a small bank of LEDs to provide some light on the cutting area. You got to love the bright LEDs and the low power requirements.

I still have a problem with chatter on the X, Y area of the cut but I am waiting to do a write up until Sean has an opportunity to run the same cut file.

Today, I cut my first job for a paying client. It is nice to get that check.

Right on! A few bucks coming in feels good! I did my first job yesterday... sweated a few bullets as the material was quite expensive!

Nils, what did you cut for the customer?

I cut a simple shape out of a piece of PVC board that was 1/4" x 4' x 8'. It took me more time to be sure I was cutting it right than it took to cut it. The material was supplied by the cutomer and so was the file that I needed to cut. They were going to pick it up but being the first client, I was happy to deliver it.

This is always the best news! :)

For the guys who havn't been in the "materials cutting" business before, it is the beginning of a path to creating a client base.

Nils did you take any pics to put in the showroom section.

Irfan,

I am sorry I did not and I wanted to but my camera needed to be sent back to Nikon to get some warranty work done on it.

Congratulations on your first Job Nils! :)

My thread is getting down in the list so I thought I would post some fish I have been working on.

Plywood just to test how they look. The last is solid surface material and it is going to be used as a Trivet.

Fish in 1/2" Cork

Interested to hear how you machined that "soft" material without distortion?

Alan,

It wasn't that hard. I called Onsrud to see what bit to use. They told me that they have never cut cork but they suggested a 63-000 series bit. I happened to have a 63-775.

I tried a small cut with my shuttle pro and it machined very nice. Sharp edges and smooth. I rounded the edges when I cut it in solid surface and the edges are rounded in the cork.

So I set up my file and cut it. The router was at 15,000 and I think the feed rate was 30 but I think it could have been faster may be 70.

I am very pleased with the results. I think I am going to make the spine a little thicker to make it a little stiffer.

Looks good in cork. I bought the cork from McMaster Carr.

Trivet for hot plates.

Hope that helps.