Acceleration and Deceleration

[GJMATHEWS]

Myself and Eric have been hitting the books. As a result of a Wincnc.ini file that Eric emailed me from his machine I was forced to take a closer look at mine. Up until a few days ago, I thought my machine was cutting very nicely. As I have stated in an earlier post, since I cut furniture, anything within 1/64 of an inch is acceptable. My photo album bares witness to the fact that the machine is truly a great piece of equipment. Just take a look at the pair of hooters I carved on it!
[lol]

I had sent an email to Eric just the day before telling him that my machine does not seem to slow down when it gets to a corner. It was his ini file that clued me in to what was going on.

During any cutting operation on any CNC machine the X and Y axis directions can suddenly change. For cabinet makers, a 90 degree corner does not pose as much of a problem as carving a 3D object. When cutting a rectangle, the machine travels along the X axis to a specific point and then makes a turn and starts along the Y axis. The process is repeated at the next corner and so on until the rectangle is cut. In carving 3D, there are usually 2 axes involved within a millisecond. In the case of spiral cutting, there can be 3 involved within milliseconds of each other. Compound that by starting from the center and working out... well you get the idea if you have been around CNC long enough. Since the computer can read ahead in the program, it knows that a corner is coming up and it will send a pulse telling the servos it is time to slow down. Rather then taking the corner at 600IPM, the servos will slow down, (decelerate) take the corner and speed up. (Accelerate)

Think of it as human being for one minute. If you were using a router and going around a corner to radius or profile an edge, you would slow down as you negotiated the corner and then resume a good cutting speed. This is what a CNC machine needs to do to function at its best.

Prepping bentwood cherry chair arms the other day, I noticed the cuts were no where close to the cuts my Shopbot was given me. It was the same file, just a different G-code. That is when I finally realized that my machine was not slowing down as it approached corners and any tight radius cuts. At the time I was cutting at 150IPM.

Because I had over 50 of these chair arms to cut, and with a little encouragement from Eric's email, I started to screw around with my .ini settings.

WARNING, DO NOT TOUCH THESE SETTINGS UNLESS YOU ARE WILLING TO RELEASE CAMASTER FROM ALL WARRANTY WORK!!!

Little disclaimer for the guys at CAMaster.

Anyhow, after making a few adjustments, about 22 to be precise, I am pleased with the results. Keep in mind that these files are for my machine and I do not make any claim, guarantee, warranty, statement, diatribe, written, spoken, or implied gesture that they will work on your machine. If you copy them and use them and wreck your machine, "Oh well!!! Sucks to be you!" They are here for you to look at and learn from. If you do use them you do it at your own risk.

All the information that I used to modify them came from the Help File located within my WINCNC Software package. Each modification was then followed by testing on my machine and solely on my machine. Please do not think that for one minute they will work on yours. I do not know what drives your machine has, what servos, what table width, length and so fourth, and so on, and yada, yada, yada.

In other words, when in doubt, consult the manual or the guy that covers the warranty on your machine. These settings have not been approved by anyone at CAMaster or Wincnc. My use of them has more than likely voided the warranty on my machine. That is a consequence that my boss and I can live with. We did not buy the CAMaster to get a warranty. We got it because it is a damn good machine and we like to push good machines to the limit!!!!

Anyway, having said all that, 3 months from now, someone will try the exact same settings I have posted here and slam their gantry into a brick wall and try to blame me. Guess what guys? I don't do guilt and I am going to die poor anyway!

In Bold are my original settings that came with my machine after we set it up and Josh and I got it going in my shop.

[Demo Mode]
demomode=0

[Timer Card Settings]
timertype=7200

[Pulse Outputs]
steppulse=p5d5
maxstepv=50000

[Smoothing]
g09=s30

[Table Size for Viewer]
table=x0 y0 w60 h120 b1

G37=g53 X102.102 y-9.794 D-2 F20

[Tool Changer]
atc1=a2

[Spindle Speed]
da=t1 v10
spindle=t2 r24000

[Axis Settings]
axischar=XYZA

[Velocity Groups]
vgroup=fxy
vgroup=xy
vgroup=z
vgroup=a

[X Axis]
axisspec=p0 s1 d1 r2546.47909 o1 e0 a1500
axisvel=r350 f1500 s50 m500 h1150 c10
axislo=p2b7

[Y Axis]
axisspec=p0 s0 d0 r2546.47909 o1 e0 a1500
axisvel=r350 f1500 s50 m500 h1150 c10
axishi=p2b6

[Z Axis]
axisspec=p0 s3 d3 r4981.862 o0 e0 a1500
axisvel=r350 f1500 s20 m50 h450 C10
axishi=p3b1
altaxislo=p3b2

[W Axis]
axisspec=p0 s5 d5 r23.529411 o1 e1 a12000 t4
[r4235.294
axisvel=r36000 f1500 s5 m20 h36000 c360

[Arc Settings]
g2modal=1
arc_err=.01

[Soft Limits]
lolim=x-.01 y-.01 a-50000
hilim=x120 y60 z0 a50000
lobound=z-0.020
softlim=T1

[Abort Cushions]
lim_cnt=1
esc_step=100
lim_step=128
lim_mode=1

[Aux Outputs]
auxout=c10p4b5o0s0 [ TOOL CHANGE ACTUATE
auxout=c2p4b7o0s0E0 [ CONE CLEAN
auxout=c3p4b6o0 [ DUST BOOT
auxout=c20p4b4o0s0x0e0 [ SPINDLE FWD
auxout=c14p4b0o0s0 [ SPEED REF 1
auxout=c13p4b1o0s0 [ SPEED REF 2
auxout=c12p4b2o0s0 [ SPEED REF 3
auxout=c11p4b3o0s0 [ SPEED REF 4
auxout=c26p7b7o1s1 [ STEP DIV GEAR CHANGE
auxout=c33p5b7o0s1x0
enab=c33

[Aux Inputs]
auxin=c1p0b0
auxin=c2p0b1o1d10
auxin=c3p0b2o0
auxin=c4p0b3o1 [TOOL TIED]
auxin=c5p0b4o1
[auxin=c6p0b5
auxin=c7p0b6
auxin=c8p0b7
AUXIN=C9P3B4o0 [ESTOP]
enab=c9m"E-Stop Pressed"t1
auxin=c11p3b5o0 [Enable Servos]

[Enables]
enab=c9m"RESET E-STOP"a
enab=c11m"RESET SERVOS"a

[G28 Settings]
g28move=z-.25 f75 t2.5
g28move=x.25 y-.25 f200 r.3 t2.5
g28coord=y60.784

[File Types]
filetype=*.TAP;*.NC;*.MAC;

With the above settings, I could not run the chair arms any faster the 175IPM's without chatter.

Below are my new settings in Italics I have highlighted changes in blue.

[Demo Mode]
demomode=0

[Timer Card Settings]
timertype=7200


[Pulse Outputs]
steppulse=p5d5
maxstepv=50000

[Smoothing]
g09=s19

[Table Size for Viewer]
table=x0 y0 w60 h120 b1

G37=g53 X102.102 y-9.794 D-2 F20

[Tool Changer]
atc1=a2

[Spindle Speed]
da=t1 v10
spindle=t2 r24000

[Axis Settings]
axischar=XYZA

[Velocity Groups]
vgroup=fxy
vgroup=xy
vgroup=z
vgroup=a

[X Axis]
axisspec=p0 s1 d1 r2546.47909 o1 e0 a1000 f150
axisvel=r800 f1500 s50 m500 h1150 c15
axismode=s19 v25
axislo=p2b7

[Y Axis]
axisspec=p0 s0 d0 r2546.47909 o1 e0 a1000 f150
axisvel=r800 f1500 s50 m500 h1150 c15
axismode=s19 v25
axishi=p2b6

[Z Axis]
axisspec=p0 s3 d3 r4981.862 o0 e0 a500 f150
axisvel=r350 f1500 s20 m50 h450 C15
axismode=s19 v25
axishi=p3b1
altaxislo=p3b2

[W Axis]
axisspec=p0 s5 d5 r23.529411 o1 e1 a12000 t4
[r4235.294
axisvel=r36000 f1500 s5 m20 h36000 c360

[Arc Settings]
g2modal=1
arc_err=.01
arc_min=.002

[Soft Limits]
lolim=x-.01 y-.01 a-50000
hilim=x120 y60 z0 a50000
lobound=z-0.020
softlim=T1

[Abort Cushions]
lim_cnt=1
esc_step=100
lim_step=128
lim_mode=1

[Aux Outputs]
auxout=c10p4b5o0s0 [ TOOL CHANGE ACTUATE
auxout=c2p4b7o0s0E0 [ CONE CLEAN
auxout=c3p4b6o0 [ DUST BOOT
auxout=c20p4b4o0s0x0e0 [ SPINDLE FWD
auxout=c14p4b0o0s0 [ SPEED REF 1
auxout=c13p4b1o0s0 [ SPEED REF 2
auxout=c12p4b2o0s0 [ SPEED REF 3
auxout=c11p4b3o0s0 [ SPEED REF 4
auxout=c26p7b7o1s1 [ STEP DIV GEAR CHANGE
auxout=c33p5b7o0s1x0
enab=c33

[Aux Inputs]
auxin=c1p0b0
auxin=c2p0b1o1d10
auxin=c3p0b2o0
auxin=c4p0b3o1 [TOOL TIED]
auxin=c5p0b4o1
[auxin=c6p0b5
auxin=c7p0b6
auxin=c8p0b7
AUXIN=C9P3B4o0 [ESTOP]
enab=c9m"E-Stop Pressed"t1
auxin=c11p3b5o0 [Enable Servos]

[Enables]
enab=c9m"RESET E-STOP"a
enab=c11m"RESET SERVOS"a

[G28 Settings]
g28move=z-.25 f75 t2.5
g28move=x.25 y-.25 f200 r.3 t2.5
g28coord=y60.784

[File Types]
filetype=*.TAP;*.NC;*.MAC;*.TXT;

With these settings, most all of them in the AxisSpec area, I was able to run the file at 600IPM.

That does not mean that the entire piece was cut at 600IPM. It means that the machine now has the ability to cut at 600IPM and produce smooth results. On a straight axis run of 60 inches, the machine will get up to speed and travel at 600IPM. As it approaches a turn, it will slow down. These settings now have my machine moving almost identical to my Shopbot when cutting the same file.

That is today's less on Acceleration and Deceleration. I am off to go carve myself an apple!

Over the next few days I will continue to modify these settings to come up with what should serve as a good starting point for most machines running Wincnc software.

Thanks for the inspiration Eric.

Youtube video to follow of the final chair arm with screen shots of 600IPM.

[Eric Mims]

looking good Guy. We'll get there soon enough. The main thing will be for people to post, "I cut super smooth cabinets using these settings" or "I found I had to adjust this to get smooth v-carves", etc.

And as far as warranty goes, seeing as how every machine (even identical machines) had different wincnc.ini files when they were setup, not sure how adjusting them could void anything. Of course, some settings would be different from the factory (settings for table size, 3 head, etc), but as we saw when we were solving the drive problem, smoothing, acceleration, and other settings were all over the place from the get-go.

Now if somebody goes and puts their axisspec F# feed acceleration at 8000, the feed velocity at 2000, well that might just void a warranty!! :D

[Joey Jarrard]

we build the machine we set them up to a standard. Eric is correct each customers ini is diffrent. the reason is each app is diffrent. we set the machines up as a defalt each machine may get a little diffrent settings due to size or configuration. a shop doing cabinets settings will not do for some one doing 3d. we love it when customers learn how to change there settings in the ini. doing this does not void anything we do ask that you back up your settings before changeing anything and to use good judgement when changing your speeds. we can not take responsibility for some one crashing there machine. but this is limited when you look in to the settings like eric and guy are doing. and as always if in doubt just ask we will help any way we can. we have some customers that keep 2 or 3 ini files for diffrent jobs. one for cabinets that will go faster and the tolarance is not as high then others for 3d work. this is the best way of doing it to me.

I know this that CAMaster has the best customers out there. you all push the limits and think outside the box. you view your machine as more than just a tool. when you feel like that it makes you want to learn more about cnc. please keep it up guys. I learn from you as much as you from me.

one of my pet-peeves is someone who thinks ok i have a cnc it is going to come here i am going to through some sheet goods on it and it is going to make me a lot of money. this is not the story at all it takes time and a wanting to learn to do this. the world of cnc is this you get out of it what you put in to it. the more you learn and apply your self the more you get out of your machine and software.

keep it up

[james mcgrew]

count me in!!

jim

[GJMATHEWS]

Here it is as promised.

http://www.youtube.com/watch?v=m9XSI2ZPwG8

[james mcgrew]

that is an excellent piece of help for me!!

thank you

jim

[Eric Mims]

nice vid, Guy! The only small correction I might add is that when the F is not present, it uses the 'A' setting, but that 'A' setting is usually set much higher since it is the Rapid speed acceleration number. Adding the F let's you specify a separate Feed speed acceleration. Thanks for pointing that out that important setting. I think most users would benefit from having a separate, slower acceleration on their feeds.

[GJMATHEWS]

nice vid, Guy! The only small correction I might add is that when the F is not present, it uses the 'A' setting, but that 'A' setting is usually set much higher since it is the Rapid speed acceleration number. Adding the F let's you specify a separate Feed speed acceleration. Thanks for pointing that out that important setting. I think most users would benefit from having a separate, slower acceleration on their feeds.

Couldn't have done it without you Eric. You were the guy that got me off my security blanket and got me playing with these settings. I know what these machines should be doing, having generated and cut so many different projects and custom programs. Manipulating the actual software to adjust the machines by themselves was just something that you got me in to!!!
My boss is also value added, he gives me the opportunity on a daily basis to push the envelope wide open.

A pat on the back for all involved is what is needed here.

[Eric Mims]

Joey,

First, hope you're doing well and feeling good.

Second, is it possible for you guys to get in touch with the Wincnc guys and get some info on a few things. I have tried emailing them about some of their settings, but I never hear anything back. I'd like a more useful description for some of the .ini settings (more so than what's in the manual, for instance, real world differences at different settings). here's a few:

more detailed explanation of g09 setting, both the S and A settings

the 'axismode' settings S and V and how they relate to the other acceleration and smoothing settings

Also, if you can find out if it is possible to add a shortcut string to the wincnc.exe shortcut on your desktop, so that you can have an icon that start wincnc.exe using one wincnc.ini file and another icon that starts using a different .ini file.

edit: also, what is the best way to change these settings in your gcode, without closing and opening the program? If I do a vcarve, then use the other head to do a cutout, I may need different smoothing or acceleration settings.

thanks,
Eric

[Angus_Hines]

Excellent explanation of Ramping. Im sure you know Guy but you can do the same thing for your Bot with the [V]R Command and not have to know any coding

[GJMATHEWS]

There is also a clear difference between ramping and acceleration and decceleration.

Ramping is a motion that is used primarily for plunging a bit into a work surface at an angle. It differs from direct plunging whereas in direct plunging the bit moves straight down into the work. With ramping, the bit moves back and forth and works its way into the work as the z travels downward to the desired depth.

The VR commands on the Shopbot are very easy to understand and use once you get a clear understanding of what they do.

As CAMheads, we need to ultimately come to a place in the road where we can have a similar plugin for the wincnc software that allows us to change these values without having to screw around with ini files.

The VR settings on the Shopbot also control the acceleration and decceleration of the machine as it approaches corners on both the x and y axis as well as on the z.

For those of you have never played with your VR on your Shopbot, I strongly recommend you look into it. You can save vast amounts of cutting time by adjusting these. The great thing about a Shopbot is you can actually adjust these while a program is running by using the Insert Command feature. :D

[james mcgrew]

joesph b and george in wilmington told us of this some time ago, long before many of you had your machines and definantly before i got my new one, i have had some conversations with kelly at wincnc about this and was hoping he could have come to greensboro and met with some of us with the economy and so forth that did not happen. the people who probably know the most about this are not so close to the actual application. from what i have seen in two years with wincnc guy, eric and some others are the closest to applicable solutions. you guys are real close i do have a

my settings are a lot like those here and i will reintroduce the axismode line and see what happens

jim

[Eric Mims]

just so you know, if you are testing files and smoothing, you can type in g09 s15 a10 (put in different S and A settings to try different things) just like that in the command line in Wincnc to try a different G09 smoothing, without having to change your ini and restart wincnc. The 'a' setting isn't required, it changes the angle used in smoothing calculations.

[james mcgrew]

i am gonna call you in a few minutes

jim

[james mcgrew]

it is always hard to tell as i am still so impressed with my machine but i just ran a three bit file with a lot of xy changes and it was smooth and fast!1

i will run the part in maple and film it as i need to run 4

all i have done so far is to add the f200 to my axis spec line

jim

[Joey Jarrard]

WinCNC is a great program and there is a lot to it. the book is very hard to read. Guy if you get me a list of questions I will get the answers to you. PM me a list of issues and i will get on top of it. I will get it to Kelly and get with him for the answers.
Joey

[Eric Mims]

joey, I sent a few questions to Jim earlier today, so make sure you get those from him if you talk to Kelly (if Jim hasn't already asked him those).

Eric

[james mcgrew]

wincnc can be contacted at

Web: Home | Phone: (304)-472-7206 | E-mail: sales@wincnc.net

jim

[GJMATHEWS]

wincnc can be contacted at

Web: Home | Phone: (304)-472-7206 | E-mail: sales@wincnc.net

jim

Yeah... about that. You see, the thing is, they want to charge people for that tech support. When I called them a few months ago, they told me that our tech support comes from CAMaster. I realize Joey has been sick and from what I can see on this forum, you seem to be involved with the tech support end of it, so I am referring back to my first post from today.
If you guys need more help, all you need to do is ask. I am more then happy to test files and run simulations, but I am not going to go through 6 different people to get information.

Some of the problems on the forum here seem to be going on for quite some time and there seems to be a lot of "he said she said".

To be honest, because of Eric, my machine is humming along. It is and has been making my company money and with the exception of a few modifications that we are making to the gantry and the belt drive on the A axis all is grand. Of course, I have also been doing this for 3 years now 5-6 days a week so all I really have to do is post process to Wincnc instead of Shopbot or Fanuc.

However, there are other people that seem to be having problems with their machines and it seems like they are having a hard time getting them pinned down. :confused:

[james mcgrew]

guy, joey and eric

check your emails

[GJMATHEWS]

guy, joey and eric

check your emails

Okay, I have 3 for Natural Male Enhancement, 5 telling me that I have won a Nintendo Wii, 72 for Generic Viagra and 2 from Jim. [lol]

Just kidding, there was nothing about winning a Nintendo Wii!

Got the download, and will read though it tonight and tomorrow. Now we are cooking!!!

[james mcgrew]

i would be scared to send you viagra!![lol]

check with the others before posting, but i am glad we are moving forward

jim

[GJMATHEWS]

Yeah Jim, I agree with you on that one.

If I get to the shop tomorrow I am going to try a couple of macros that I stole from my FANUC Macros files.

[james mcgrew]

eric today i was running a 3d file that had a lot of arc moves in 2d when using the off set instead of raster path, i saww chatter in the curves as there were several in each section of the file. i stopped machine and changed g09 to s30 and man what a difference i also added f150 to ini and may remove it to see the difference, slowed a bit but incredible quality

jim

[Eric Mims]

Sounds good Jim. The key is to find out what settings get you good smoothing, yet don't lose any steps. Like I told you the other day on the phone, I need to run some more 3d files again to see if my Z loses steps when the G09 is high. The last time I tested this, I did not have an F acceleration setting, so it's possible that my A acceleration was too high and causing the missed steps as opposed to the G09 setting.

[james mcgrew]

i wanted to do a follow up, using "normal" wincnc spec settings and simply learning which go9 sttings work for different applications has been succesfull for me for the most part i just leave it on go9=s15

jim