Manufacturing Information Solutions Forum Index Manufacturing Information Solutions
Your Place for Support and Discussions
 
 FAQFAQ   SearchSearch   MemberlistMemberlist   UsergroupsUsergroups   RegisterRegister 
 ProfileProfile   Log in to check your private messagesLog in to check your private messages   Log inLog in 

Some helpfull Tips

 
Post new topic   Reply to topic    Manufacturing Information Solutions Forum Index -> Machining
View previous topic :: View next topic  
Author Message
John_B
Frequent Poster


Joined: 03 Jul 2004
Posts: 56
Location: Milwaukee, WI USA

PostPosted: Sat Jul 03, 2004 11:03 am    Post subject: Some helpfull Tips Reply with quote

I have accumulated these over the years, and this is as good a place as any to store them so I can find them when I need them, and i can shaire them with you also.

John



-try inserting an M19 when the tool goes home, this orients the spindle on the way up instead of when you call up M06, this saves about 2-3 seconds for each tool.

-if you need to machine both ends of a part while your holding it in a vise, and you also need a stop try using one of tools for the stop, just take 1/2 the dia. of the tool +1/16 and add this to your program, this way you can bump the part against the tool, press cycle start and the tool/stop moves out of the way! I usually use the center drill for this

-some cad/cam systems end up adding unneeded x,y or z values to the final toolpath which adds up to alot of excess code, try using subprograms for like moves in a 2D plane

- mirror image works great for producing right and left hand parts, but watch out when machining the mirrored part, if you've programmed the first part using G41 and climb milling, make sure you add at least an extra .01 to the rough cutter, because on the mirrored part you'll be conventional milling where the cutter tends to dig into the finished surface.

- if you use those seco face mills with the square inserts (t-25) why not consider the left handed model, that way when the inserts wear out on the right hand side you can still use the left hand side, this can cut your insert costs in half.

- when you need to cut a precise angle on a part, set it up in the machine with a protractor and then write a program to follow the angle with an indicator, this way you can bump the part around while the your machine is indicating.

- if you have to machine small parts with the 4th axis, but the size of the table gets in the way, try making a collet fixture thats about 5" long, this way you can hold the parts, and your also far enough away from the table to use conventional tools.

- got a thin sheet metal job that you have to drill thru so that you can fasten it on a fixture to machine around?don't bother with hold downs or parallel clamps, simple vise grips work great.

- thread milling? no problem, just remember to use the shortest possible solid holder you can find, I've tried using collets and they seem to allow the tool to chatter to much for my liking.

- does it seem like it takes forever to drill deep holes with your machining center? try this out, in your parameters you can change the amount of retract that your machine uses when its pecking, some machines use .1 to .05, that means that the machine is cutting air for .1 to .05 each time it pecks, I've sucessfully used a .01 to .015 retract in most materials on a vertical, with a horizontal you may be able to use even less.

- have you ever programmed an angle and you weren't sure if the machine was cutting that angle, so you got your protractor out to check it? don't bother with the hand tools, just go to the position page, press feed hold and divide the x distance to go by the y distance to go, 2nd function tangent, ***note*** i always check the angle at the beginning and the end of the cut. try it out, program a 45 deg. angle, the x and y distance to go should be equal.

- this one doesn't really qualify as a tip but I've seen this used so often that maybe it will help someone. when you are using cutter comp (G41,G42) the idea is to have the machine compensate for the tool dia. in other words if your cutting a 2" dia plug you program G41 H51 x1.0 (where H51 is the tool dia. offset) now you can use any dia. cutter (provided that there is enough room to move into cutter comp) the way that i see many companies program is like this, for the same 2" plug and a 3/8 end mill, G41 H51 x1.187 (where H51 = 0 for an on size end mill) i think this type of programming defeats the entire concept of cutter comp, because now your adding .187 to every point on the print.

- if your going to use one on draps, (combo tap drill and tap) on your machining center i'd make sure to spot or center drill the hole location, the length of the tool tends to leave it walk .01 to .015 if there is not a spot drill.

- during these chilly mornings in the northeast i've noticed that the first 2-3 parts, sometimes don't machine like the ones the night before, it probably has something to do with the machines being cold, what I tell operators to do is write a short program to make the machine move around in x,y,z and a and put an M99 at the end, this way they can press cycle start, get a coffee and the machine just keeps running the program over and over until the operator gets back.

- progressive fixturing? whats that? Thats the ability to make finished parts, no matter how many setups are involved, instead of doing the first operation on a 1000 parts than the 2nd, 3rd, ect....you figure out how to fixture or hold down parts in sequence so that a finished part is produced at the end of a cycle, not only does this save handling time, it also allows you to detect machining problems before they become a major headache, it take a lot of extra figuring but pays off in the long run in a big way!

- this tip brought to us by Daniel Page, its a macro program for offsetting the work coordinate to any degree by simply inputting two values, W the work coordinate and B the degrees. load this program in your memory, then call it up in a main program like this;

G65 P8010 B(value) W(value);

:O8010( INDEX SUB ROUTINE)
( WITH AUTOMATIC TRANSFER OF )
( WORK OFFSET )
(G65 P8010 B.. W..)

IF[#23LE54]GOTO5
IF[#23GT59]GOTO5
IF[#5221NE0]GOTO1
IF[#5223NE0]GOTO1
GOTO4

N1
#101=[#5221*#5221] (X)
#102=[#5223*#5223] (Z)
#103=SQRT[#101+#102](TAN)
IF[#5223NE0]THEN#104=ATAN[#5221]/[#5223]( DEGREES)
IF[#5223LT0]THEN#104=[180+#104]
IF[#5223NE0]GOTO3
IF[#5221LT0]THEN#104=270
IF[#5221GT0]THEN#104=90

N3
#108=[#2*[-1]] (INVERSE DEGREES SIGN)
#107=[[#23-53]*20]
#105=[#104+#108]
#106=SIN[#105]
#[5201+#107]=[#106*#103] (NEW X)
#106=COS[#105]
#[5203+#107]=[#106*#103] (NEW Z)

N4
#107=3D[[#23-53]*20]=20
#[5202+#107]=3D#5222 (Y)
GOTO6

N5
#300=1(ILLEGAL WORK OFFSET)
N6M99


- how about some starting points for speeds and feeds in 1018 CRS:
1/2 rough cutter 1000 rpms, 7.5 ipm 3/8 depth
3/4 rough cutter 875 rpms 7.0 ipm 1/2 depth
1/2 drill 800 rpms .125 peck 10 ipm
3/4 drill 600 rpms .2 peck 5 ipm no pilot
3" carbide face mill 6 insert positive rake 800
rpms 24 ipm .125 depth
1/16 slitting saw 4" dia hss 250 rpms 5 ipm 1/8 dp.
1/2 carbide ball, mold cavity .010 side cut
4400 rpms, 125 ipm.

- if your machining center has ever picked up the wrong tool because the counter lost count, you know what happens, crash, thats because the tool will be using the wrong height offset, you can eliminate this problem by inserting the tools into the magazine, longest tool first and shortest tool last, I know you can't do this all the time, but its one less thing to worry about when you can do it.

- fixturing material? everyone has there own preferences, so I'll give mine, t2024 alum. seems less gummy and more stable than 6061, and machines easier than 1045 crs.

- G04 is a dwell command, some use it when grooving, some use it when c'sinking holes, but sometimes if you have a good operator that you trust you can use it for simple programs that require alot of loading and unloading, as an example, suppose you have to spot the location of a hole in a 1000 parts, you can program at the end: G04 P7000; M99; this gives the operator 7 seconds to unload and load a new part, without ever having to touch the cycle start button, true it can be dangerous, but it sure beats pressing that green button!

- plastics, there easy to machine but can present problems when trying to hold them down, ream, or hold close tolerances, here's my advice, first use dead sharp tools, any nick or roundover is pushing not cutting, next try roughing everything and remove from vise or fixture, then do finishing with the slightest pressure possible, and last coolant, make sure you got lots to remove chips, 2-3% mix would be good.

- here's the way that i like to test out new programs; after i finish writing the code, i save the program as a file then make a copy, in the copy i change all the feed rates to F100.0 and then change the Z moves by 2 decimal places (.125 is .00125) and (2.375 is .02375) then i download to the machine tool, now you can check the program without having to use dry run and your also only skimming the top surface of the part. If everything seems in order you can delete the copy, download the original and start making parts!

- vertical machining centers work great for lots of jobs, but the one thing that always gets in the way is the cutouts that are sometimes left behind after a machining operation, sometimes you can bolt thru to hold them down, other times you can just mill the cutout away, but the easiest way around the problem is to just mill clearance holes, or pockets thru the fixture and leave the cutouts drop thru.

- I just learned this tip this week, while programming a cam profile I used the part line as the basis for the program using cutter comp,(G41)(G02) the part came out lumpy, so I went back and programmed the cam follower line instead and comped off of that line (G42)(G02),the part came out smooth, in both cases the part was being climb milled. I don't know why but I think it has something to do with the greater apparent shift between points. In other words,picture this, mill a 4" circle using G41 and a .5 end mill:

G00 G90 X0 Y2.75
G01 G41 D51 Y2.0
G02 J-2.0
G01 G40 Y2.75
D51=.25
now........
mill the same circle using G42 and a 1.0 offset
line
G00 G90 X0 Y2.5
G01 G42 D51 Y3.0
G02 J-3.0
G01 G40 Y2.5
D51=.75

the machine thinks its using a much bigger cutter than it really is, hence, the greater apparent shift between points.

- if you still have to manually input you're programs at the machine control, you can save yourself considerable time and keystrokes if you write small sub- programs for code that repeats over and over, for example;

GOOG90Z.1
M09
G80G00G49G28Z0M19
G28G91X0Y0
M01


just list that code as a sub-program and call it up at the end of each tool, now you can return to the reference point, turn the coolant off, cancel the tool length, cancel a canned cycle and orient the spindle all just by calling up M98P---- sure saves alot of manual input!

- ever try to pick-up the edge of some 4140 tool steel after heavy milling and the edgefinder starts going crazy? its probably because the part became slightly magnetized, you can pick-up the edge accurately with a 1" standard of brass or alum.

- this might seem like common sense, but I've seen it occur so often that i thought it was worth mentioning, when your milling a slot with cutter comp and the end mill goes around the radius it seems to feed faster then when its doing the straight move, hence the width of the slot is good but the length isn't quite there, what i do is program a feedrate in the corners thats about a 1/2 to a 1/4 what the feedrate is for the linear move.

- If your making a milling fixture to hold down parts, the best way to go about it is to mill bosses instead of just straight tapped holes that way you only need minimal downpressure to hold the work securely.

- did you know that you can use negative offsets on machining centers to make an inside and outside part using the same program, you can just make sure you have enough room to move into cutter comp.

- here's a fairly good program for spiraling down to rough a 4" hole 3" deep for finish boring, (I only use this program for deep holes, 3-6")


O0001
G00G90X0Y0S995M03
G43H01Z.1M08
G01Z0F100.
G41H51Y2.0F25.
M98P300002
G03J-2.0
G01G40Y0
M09
G80G00G49G28Z0M19
M30

O0002(SUB FOR SPIRAL)
G91G03J-2.0Z-.1
G90
M99


- if you have a part that needs milling done all around you can leave the stock about a 1/4" over and use that to hold in the vise, then when the machining is done you can use a face mill to mill the excess off.

- a young man e-mailed me a question about small hole drilling, he wanted to know a good starting point for a .010 drill .075 deep in 304 stainless, 300 holes per part, fortunately, I had recently done something similar so heres what I told him, speed 3400, use a G83 instead of G73, peck Q.005, feed .2 ,retract .005, I was able to drill 225 .013 holes with these parameters, this may not be the optimum set-up according to some books but it does work in real life situations.

- did you know that you could use your edgefinder as a poormans digitizer, to define the shape of a 2D part for which there is no print, just walk around the part with the edgefinder and record the coordinates then put them into a cad system and connect them to get the shape of the part, now you can make a program to cut that part, don,t forget to subtract the .100 for the edgefinder.

- Need to mill a narrow width slot thats fairly deep, try this: first drill your pilot hole, then use an end mill that has the same diameter shank as the cutter, extend it out of the holder only as much as needed, now G73 to depth, say 1.25", then G80 to cancle that drill cycle, now go to a sub program using G81 to depth at 25 to 30 ipm and a G91 move for increments of cut, say .005 or .010, loop this subprogram as many times as need to make the lenght of the slot: Sample program for 1/4 slot x 1.25 lg in A-2 tool steel, this program worked to hold slot straight and a tolerance of .250 +.002/-.000 and a 63 finish

MAIN PROGRAM
O5000
G00G90X0Y0S2500M03
Z.1M08
G73G98R.1Z-1.25Q.125F10.0
G80
M98P1005001
M09
G80G00G90Z5.0
G28G91Y0M05
M30
SUB
G81 G98 R.1 Z-1.25 F30.0
G91 X-.01
G90
M99
Back to top
View user's profile Send private message Send e-mail
Display posts from previous:   
Post new topic   Reply to topic    Manufacturing Information Solutions Forum Index -> Machining All times are GMT - 5 Hours
Page 1 of 1

 
Jump to:  
You cannot post new topics in this forum
You cannot reply to topics in this forum
You cannot edit your posts in this forum
You cannot delete your posts in this forum
You cannot vote in polls in this forum


Powered by phpBB © 2001, 2005 phpBB Group