New Z Slide Going In! #12 - Winter Park, FL

[gmessler]

The space for working must be sooooo nice!

[sailfl]

Greg M

Are you talking about the space in my box? I had most of the wiring done outside the box and then place the plate in the box. I wired the motors, proximity, power, router and door switches as the last thing and they did not require much.

It is a big box. Heavy!

[sailfl]

I didn't just work on the problem.

This is a rough cut but I will share it with you. I cut a file that came with the software of some grapes recessed. I did a rought cut with 1/4 end mill and another relief cut with a 1/4 ball nose. I set the ball nose too deep so it cut deeper than it should. But I am learning.

Also the material is cabinet plywood so it is not the smoothest cut. I am happy with what I did.

[sailfl]

Having worked on building the machine for 6 months, it is fun just watching it cut a simple file in a scrape piece of cabinet plywood and having it turn out really nice. I need to use one more bit and do a final cut to get a smoother finish but I am impressed with the way the machine does it thing.

[gmessler]

Looks Great Nils,

What software did you use?

[sailfl]

Greg M,

I have a borrowed copy of ArtCam which I will most likely not be buying only because of what it cost. I have not decided what I will end up with. I like Aspire and I am starting to consider Rhino and RhinoCam. I am still in the learning mode and I am not sure what my needs will be.

I was pleased with the cut. I am going to cut the same image in a hardwood and finish with a 1/8 ball nose which I did not do on the cut. I think it will clean it up even more.

[domino11]

Nils,
Do the grapes come with artcam or did you get them somewhere else?

[sailfl]

Heath,

Part of the files that came with ArtCam.

[Kobus_Joubert]

What is the size of those grapes and how long did it take to rough and how long for the final cut ?

[sailfl]

The size is 4" x 12". The rough cut took about 25 mins and the relief cut took about 20 mins.

I will pay more attention to cutting information but it took 3 passes with the 1/4 end mill and 1 pass with the 1/4 ball nose. I have my Milwaukee set at the 3rd setting for the speed. I think that is 14,000. I looked and the feed rate for each of the bits is set a 100 IPM.

I am just happy to watch it cut. As I mentioned, I am going to recut the same file in a piece of oark since I have it in my garage and use three bits. I have been using a carbid tipped 1/4 end mill and I think I will use a solid carbid though the performance I think will be the same but maybe a better cut. I will use a 1/4 ball nose and 1/8 ball nose.

One other note about the Milwaukee router. At the 3rd setting, I do not need to wear any ear protection because the router is so quiet. I am going to start wearing it any way for added protection.

I will post another pic.

Gerald, there is small amount of saw dust collecting on the machine and floor. No more clamps cut.

[sailfl]

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.

[normand blais]

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

[javeria]

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

[sailfl]

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.

[javeria]

Originally Posted by sailfl

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

[Gerald D]

Originally Posted by sailfl

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.

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

[Greg J]

Nils,

Onsrud has great technical articles and information.

https://www.onsrud.com/

[sailfl]

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?

[bradm]

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.

[Gerald D]

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.

[sailfl]

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.!

[YRD]

Nils,

Follow Brad and use the G61.

[Gerald D]

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 . . .

[sailfl]

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?

[bradm]

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:

Program G61 to put the machining center into exact path mode, G61.1 for exact stop mode, or G64 P- for continuous mode with optional tolerance. G61 visits the programmed point exactly, even though that means temporarily coming to a complete stop. G64 without P means to keep the best speed possible, no matter how far away from the programmed point you end up. G64 P- means that it should slow down as required to keep no more than P- away from the programmed endpoint.

[YRD]

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

With the G61.

[YRD]

Brad,

Test says the G64 the corners became more rounded.

Correct ?

[bradm]

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 ...

[Gerald D]

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.

[sailfl]

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
%