JWK42
Modified the program.
Not sure I have the angle correct. I converted the X distance / part circumference X 360 to get the angle.
JWK42
Modified the program.
Not sure I have the angle correct. I converted the X distance / part circumference X 360 to get the angle.
Erm.. how about using an old drill bit (the shaft part obviously) and some aloxite and water to hand grind the chamfer- if you aint got that then use Valve Seating Abrasive. Note when grinding like this nice slow movement and constant but medium pressure works best. Take the shine off the drill shank first by sticking it upside- down in a drill and hand grinding with a 2"X1" thin sheet of aluminium and aloxite. Wash with soapy water.
Would take you about 5 mins per hole and could be done while the next part was being machined.
Hell, it's only to make it look nicer... hand chamfer it.. you can say in your company literature "Hand Finished by Professionals"
Iain.
[Edit]If you can't get the proper abrasive then goolge "Jeweling abrasive" or "Engine Turning"- the kits sell for about 6 dollars on E-Bay I beleive [/Edit]
I love deadlines- I like the whooshing sound they make as they fly by.
Kiwi
I did this about 20 years ago for our Maho mill with rotary table but no cylinder interpolation. I created a points file every 1 degree for a 4 inch dia circle. I then used the X value of each point as Opposite and the 22 inch radius of the cylinder as the Hypotenuse to calculate the degrees of rotation for each point in Y axis. The result generated a good chamfer on the hole.
But doing this by hand 90 times then cutting and pasteing and changing the signs to create a 360 point file was a big pain.
In the examples below of your file and the OP/HY method I used the A points are very nearly the same. I am not sure which points correct but a few hundredths of a degree won't matter for most parts.
I would like to see the code use G01 in the first line only.
I would like to see whole number like this Y2.
I would like to see the A formated to 3 places instead of 4
G01 Y0. A5.209
Y0.291 A5.180
Y0.5176 A5.031
Ex. from your file
G01 X0 Y0 Z0 A5.2087
G01 X0 Y0.2091 Z0 A5.1802
G01 X0 Y0.5176 Z0 A5.0312
Y0.684 A4.8946
Y0.8452 A4.7207
Y1 A4.5109
Y1.1471 A4.2667
Y1.6961 A2.7602
Y1.9225 A1.4357
My calculations
use X point from the 4 in dia point file as my OP and use 22 in as my HY
to find degrees
X2.00 = A5.216
X1.989 = A5.187
X1.9319 = A5.038
X1.8794 = A4.901
X1.8126 = A4.726
X1.7321 = A4.516
X1.6387 = A4.271
X1.0598 = A2.761
X.5513 = A1.440
I couldn't get this thing to leave the columns beside your examples but I think you can follow what I have done.
Thank you so much for sharing your work
JWK42
As a slightly off-topic comment. This reminds me of the old-fashioned apprenticeships that required the apprentice to spend weeks hand filing a square hole and plug to a fit of a thou or two.
It works but I am glad there are alternative ways.
P.S. Fortunately my boss when I apprenticed saw no merit in teaching me the slow way to do something so I never did the filing bit.
An open mind is a virtue...so long as all the common sense has not leaked out.
Kiwi
I just wrote a Macro program using SIN & COS for our Haas simulator that lets the control calculate amd mill through the 360 X-Y points of a 4 inch circle. I didn't attempt to calculate the Z moves. It took 10 secs longer to calculate and run the circle points than to run the points down loaded from my PC. Not a big difference in time to mill 12.566 inches at 12.566 fpm
JWK42
The math for a simple path along the edge of the hole shouldn't slow the CNC to any noticable degree.
I'm working on getting a tool path for a ball nose cutter to cut the chamfer with a consistant width and bi-secting the two face angles which will slow a CNC.
I've modified the program as requested.
The X axis has been changed to A Rotation. Should this not be B running along the Y axis?
Please put me right.
ImanCarrot
I get a number of parts to make which require a chamfer around the edges which is for appearance only. This detail makes the part look good.
Chamfering a hole is no different when the machine is able of doing this.
I guess most people just put it in the too hard basket.
Toby D.
"Imagination and Memory are but one thing, but for divers considerations have divers names"
Schwarzwald
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
www.refractotech.com
Kiwi
We're running Haas HMC's and they use 'A' for all 4th axis rotary tables.
Our 1985 Maho is being repalced in about 3 weeks. It used 'B' axis for rotary.
The decimal after whole number is also a Haas thing.
Your new output looks great.
One more thing!!
Can you allow me to save the points file to the hard drive after it is generated. Cutting and pasting is cumbersome but can be done.
On Chamfer#3 and now Chamfer#4 the box runs off the bottom of my screen and I can't copy all the points at once.
Thanks again.
JWK42
070808-1400 EST USA
Kiwi:
If your CNC has a math coprocessor, high speed processor, or multiprocessors, then you may not notice the calculation time in machine execution.
However, without the math coprocessor being used I believe you will find substantial delays at any reasonable feed rate.
Are you aware of how trig functions are calculated? These take a lot of processor time.
If you do all the point calculations external to the CNC and just send points, then your source file is big.
.
Copied from from an earlier post---
I just wrote a Macro program using SIN & COS for our Haas simulator that lets the control calculate and mill through the 360 X-Y points of a 4 inch circle. I didn't attempt to calculate the Z moves. It took 1 min & 16 sec to calculate and run the circle points. It took 1 min 6 sec to run the 360 points down loaded from my PC. Not a big difference in time to mill 12.566 inches at 12.566 IPM.---
Just ran the same program using 3600 points and it takes 3 min 13 secs the 1st time through and 2 min 46 secs to calculate each point after that instead of 1 min 16 sec for 360 points.
I also downloaded a file with 3600 points from my PC and it takes 1 min 9 sec to run that file.
So I guess it does slow down processing when there are more points.
I noticed that the control runs each file faster after the 1st time through, so it must be cacheing or something like that.
The 3600 point file is 61912 chars long however.
Do you have a Haas machine with HSM? I have been told that the HSM option allows macros to run faster and yours would be a good test. If you don't have HSM do you mind posting your macro; I have two machines about the same age on with HSM one without. I could do a dummy run on each and compare.
An open mind is a virtue...so long as all the common sense has not leaked out.
JWK42
You can move the curser over the code text, RH click and select 'Select All'
I can get the file saved to notepad but notepad needs to be in a known place. Usually I put a copy in C/Windows folder.
I think I will alter the program so axis letter can be nominated.
gar
OK. These files the program generates don't have anymore than 360 blocks (lines)
Do it by Hand. Use an old drill bit (bout4mm dia), abrade the bit surface (the non spiraly part obviously) of it so it goes "grey" using light abrasive and 2mm thick ally plate 2"X1"XThin with skill...
Then, use skill to manualy chamfer it.
Abrasives are gonna be here for cheap.
"Jeweling" or "Engine Turning".-------- G THAT (as in Google) if you need the abrasive.
It will take you about 5 mins to do each chamfer. Do it when the next part is running.
Say on your Company Brochure...
"Hand Finished by Experts. Why expect less than Total Skill."
I should be in advertising!
Gimme money lol- Iain.
I love deadlines- I like the whooshing sound they make as they fly by.
070808-1852 EST USA
Kiwi:
True only 360 lines in this one case. Make it 100 holes and it is 36,000 lines. Or do multiple passes and the number is proportional to the number of passes.
Create a general subroutine with a few parameters and there is not much expansion in code, but at the penalty of calculation time. In older machines it will not be as fast as your simulator.
.
Take a look at this site.
The easiest way to chamfer an uneven hole is to use a Heule Cofa.
I use them all the time and it works well.
You use it mainly for deburring but it can be used to chamfer also.It all depends on how hard you set it.
http://www.heule.com/default.asp?h=1...=68&s=2&un=128
gar
OK, I understand what you are saying. I would probable use G53/G54 for multiple holes. Large files are not a problem for me to run.
Having a program to generate the code is far more convenient as far as I'm concerned. I don't need to study the math formula to get the tool path correct and can be done in the office while the machine is working.
JWK42
Altered program to enable save to notepad.
Kiwi
Thanks so much. The output is exactly the way I wanted it. And jumping to Notepad works great. I can save the file where ever I need to.
Geof
Below is the Macro I used to run the test. I just removed the line N400 and changed N380 to G01 X#624 Y#625 F12.566 to mill the 4" dia circle in 1 minute with no lag in calulations.
So I just machined between the points. I ran this on our simulator, it is susposed to run real time
We don't have HSM yet. The Haas VF-3YT coming in a few weeks has it as part of the option package.
%
O3544 (MILL HOLES ON A B.C.)
N30 (WRITTEN 07-24-2007 14:57:49)
N40 (MODIFIED 08-09-2007 07:29:31)
N50 #602= 1.125 ( DIAMETER OF HOLES )
N60 #603= 4.0 ( BOLT CIRCLE OF HOLES )
N70 #604= 0.2 ( DEPTH OF EACH MILLING PASS )
N80 #605= 3.0 ( NUMBER OF MILLING PASSES )
N90 #601= 7.0 ( FEED RATE )
N100 #620= 3000.0 ( SPINDLE SPEED )
N110 #606= 0.5 ( DIAMETER OF END MILL )
N120 #621= 83.0 ( PERCENT OF END MILL DIA STEPOVER )
N130 #607= 3600.0 ( NUMBER OF HOLES )
N140 #608= 0.0 ( STARTING ANGLE 3 O:CLOCK = ZERO )
N150 #609= 0.1 ( DEGREES BETWEEN HOLES )
N160 #610= 0.0 ( TOP OF PART IN 'Z' AXIS )
N170 #611= 2.0 ( CLAMP/FIXTURE 'Z' AXIS CLEARANCE PLANE )
( END OF INPUTS )
N190 #604= [ #604 * -1 ]
N200 #612= [ #602 / 2 ]
N210 #613= [ #603 / 2 ]
N220 #616= [ #606 / 2 ]
N230 #617= [ #606 * [ #621 / 100.0 ] ]
N240 G17 G54 G90
N250 G40 G49 G80
( TOOL #01 IS AN END MILL )
N270 G53 G00 Z0. ( RESTART TOOL #01 HERE )
N280 G53 G00 X-20. Y0.
N290 T1 M06
N300 S#620 M03
N310 #618= #608
N320 #627= #607
N330 #624= [ COS[ #608 ] * #613 ]
N340 #625= [ SIN[ #608 ] * #613 ]
N350 G54 G00 G90 X#624 Y#625
N360 G43 Z#611 H01 D01 M08
N370 WH [ #627 GT 0 ] DO1
N380 G00 X#624 Y#625 (changed to G01 X#624 Y#624 F12.566)
N390 Z [ #610 + 0.1 ]
N400 M97 P500 (removed this line)
N410 #627= [ #627 - 1 ]
N420 #618= [ #618 + #609 ]
N430 #624= [ COS[ #618 ] * #613 ]
N440 #625= [ SIN[ #618 ] * #613 ]
N450 END1
N460 G53 G00 Z0. M09
N470 G53 G00 X-20. Y0.
( UNLOAD HERE )
N490 M30
N500 ( START OF HOLE MILLING CYCLE )
N510 G01 Z#610 F#601
N520 G13 G91 Z#604 I#616 K#612 Q#617 L#605
N530 G90
N540 G00 Z#611
N550 M99
%
WOW, these will come in handy!!!!!!:rainfro:
Toby D.
"Imagination and Memory are but one thing, but for divers considerations have divers names"
Schwarzwald
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
www.refractotech.com