Eng-Tips is the largest engineering community on the Internet

Intelligent Work Forums for Engineering Professionals

Register Log in
  • Congratulations waross on being selected by the Tek-Tips community for having the most helpful posts in the forums last week. Way to Go!

i feel the need the need for speeds and feeds !! 2

Status
Not open for further replies.
eski1

eski1

Mechanical
Jun 15, 2004
90
0
0
GB
hi just wanted to know if there is a web site that has useful speeds and feeds tables for machining stainless steel , steel , aluminium and brass these are for use with both a vertical cnc mill and a cnc lathe max rpm 3000 on both . Bascially are machining department is going through alot of tooling and i think a few laminated charts reminding them of the speeds and feeds and if possible how deep a cut to take wouldn't go a miss . Both machines work in mm/ minute and rpm to it would be helpful if the charts were in this
thanks in advance for any response
cheers chris
 
Replies continue below

Recommended for you

Sort by date Sort by votes
hi thanks for replys so far , the program you told me about is great . Does anyone know if there is any sheets that i can print out and laminate on the subject
cheers
 
Upvote 0 Downvote
I got some good charts from our OSG rep the last time he came by, and they were even already laminated too. I went over to their website and unfortunately it is worthless. If you deal with OSG at all I am sure they would fall over themselves to help you out with speeds and feeds charts.

Not to go a little off topic but this is something I have never understood. I see the OSG guy maybe once a month or even less and he is extremely helpful and gives me everything I need and ask for. I surf over to their website looking for simple speed and feed info or other basic info and I run headlong into a mountain of complex mumbo jumbo and double talk that only prevents me from finding what I am looking for!!!!!!

I just needed this time to rant a little. Thank you.
 
Upvote 0 Downvote
I figure here is the best place to post this, as I don't think it would go over to well to start another thread on it.

Anyway, I'm the in-shop CNC Programmer/Operator trying to figure out how to use an ancient Thermwood CNC Router--No graphing functions, no direct loading of programs from the control software (all transfers have to be done in DOS Mode and then rebooting of the control software), and some rather unusual G-code settings (G53.x is the tool/part offset code?! There is no subroutine coding?!)to machine an unusual plastic material for the parts on this page:


A picture which will give you a general idea of what I'm making is in the top right corner of the page, and there is some technical data on the plastic material itself if you scroll down.

Anyway, the only discernible limitation I've run into is that the RPM speed must be a minimum of 1,800 RPM but no more than 20,000 RPM--Table feed rates can range from 1-1,000 inches per minute, though I've never taken it above 300 because of the resulting vibration from the motors making me quite nervous about it maintaining any degree of precision in it's movements.

My current dilemma: I'm having to cut about 156 "herringbone" pattern slots in a single part with a 1/2" diameter carbide end mill (30 degree helix, 2" length of cut and 4" overall length of the tool, with about 3" of it hanging out of the spindle in order to avoid crashing into the monstrous clamping system I'm forced to use) at about 1.250" depth per slot, those of you reading this who work with similar machines can probably guess at what kind of problems I'm running into in terms of tool vibration at higher speeds... but the best I can come up with is about 3,000 RPM/36 Inches per minute.

Which is, of course, unacceptable in terms of production time as the order calls for 7 of these parts, and our ever-zealous sales staff agreed to a deadline of October 6 for the shipment.

So... can anyone here offer any suggestions in terms of alternative tooling for this problem?

Also, are there any freeware programs out there that can convert an AutoCAD drawing to NC Code automatically?

I'm wasting inordinate amounts of time programming these things in notepad and copying them directly into the hard-drive of this CNC machine, testing the program without tooling or on scrap material to make sure I haven't made any errors in these several hundred line programs.
 
Upvote 0 Downvote
A minor edit, the CNC Router is a 3-axis "gantry" type--the bit travels around on a boom above the table as opposed to some others I've seen where the bit is stationary and the table moves about.
 
Upvote 0 Downvote
You are now feeling the pain that old-timer programmer felt about paper or mylar tape which was manually punched and manually corrected.

I am assuming the 156 slots will be identical and the moves will just be indexed by some amount for the length of the part. Program the first slot and create a spreadsheet using columns for the various codes areas N,G,X,Y,Z,I,J,K,F,S,T. Do not enter the values that are indexing with the code letter enter the NUMBER only. Create your second slot but instead of copying and pasting the indexed values add the indexing value to the previous locations. Then cut and paste the second slot 154 times. Insert a column next to the number column. Create a formula with the proper prefix and the number value; example =if(B23="","","X"&B23). Copy the formula down the column. Cut and special paste values to get rid of the formulas. Delete the orginal number column and save the program as a .txt flie. Use notepad to take care of any other editing.

Reduce the tool overhang by changing the clamping if possible. Use serrated edge clamps to remove anything above the part. Carrlane is one manufacturer of this type of clamp.

I once saw a manually written program for milling kidney slots (1/2" wide slots on an arc) in a hydraulic pump body. The machine was a point to point vertical machine which did not have linear or circlular interpolation. They used short point to point chatter routine to mill the slots. There was about 400 points in each slots and to top it all. The coordinates were calculated using a trig table. This was preceded scientific calculators. The tape was punched by hand and verified by hand.

You do what you have to do to get the job done.
 
Upvote 0 Downvote
A great free backplotter, Discriminator, is at . I like it so well, I use it professionally.

It's a trial version, but doesn't time out and is only disabled in unimportant ways. It's also a CNC editor, so you can program interactively.

To convert DXF to G-Code, look at Ace Converter. It's free. I haven't used it, but have read good things about it.




Manufacturing Freeware and Shareware
 
Upvote 0 Downvote
Heh, I've finished the CNC portion of that order already, thanks, though. It turned out I just had to "tweak" the spindle speed down to 2,500 RPM to get the majority of the vibration out of the tool. And I'm already using a serrated end-clamp setup w/a fence on one side of the part to hold the part down/in place. From a programming standpoint as far as positioning went, it was a relatively simple part--I was just having problems with the feed/speed aspect of it because of the length of the tool I was having to use in order to get the depth I needed for each of the cuts.

And thanks for the links to the programming tools, I'll definitely be giving them a look-over when I get to work in the morning (I sent a link to this page to my workstation at work).

My current project now involves a similar part, except that it is one continuous slot that is a series of linear/circular interpolation moves--with sloped "landings" at specific locations throughout the slot in order to provide support for the part so I'm not just cutting the thing in half.

...these 800+ long lines in manual coding are giving me headaches. :D

The urge to save humanity is almost always only a false-face for the urge to rule it. -- H.L. Mencken
 
Upvote 0 Downvote
Did anyone else here notice that you could produce a kind of spiral cut if you tack codes like:

G90G1Z.6

or

G90G1Z-.6

On the end of a line like:

G91G17G75G2X-2.75Y-3.5R1.0

NOTE: The coordinates were just an example, I have not made sure they'd actually work in terms of the radius passing through the two given points in the X or Y values.

?



The urge to save humanity is almost always only a false-face for the urge to rule it. -- H.L. Mencken
 
Upvote 0 Downvote
"You might evaluate the use of incremental subroutines to cut your coding down. Easy to lose track of where you are, but very nice once you get them worked out."

I use "subroutines" of sorts, except this machine forces you to write a seperate program and reference it in your main program with the M98 word and the L variable to tell it how many times to repeat it.

Also, new problem. My machine has ceased to recognize the R variable when I'm attempting to do circular interpolation, and I'm writing a subroutine so I can repeat a series of irregular arcs. It isn't because the radius is in multiple quadrants, I've already specified the G75 code earlier in the program...

I believe that the ancient hardware driving my machine is getting ready to go.. :D

I'll try obtaining the I and J variables and changing my program again, but it kills me to think I'll have to go through all the old programs I've got and do the same thing...

The urge to save humanity is almost always only a false-face for the urge to rule it. -- H.L. Mencken
 
Upvote 0 Downvote
Most machining centers read G90 and G91 as absolute or incrimental mode of moving or cutting and can not have both in the same line. The spiral cut is useful in hogging out a pocket and is used in a couple of threading cycles. Probably some other uses I'm not aware of.
 
Upvote 0 Downvote
Yeah, I just ran into that problem, and took the second positioning code out of each line, and calculated my linear Z positioning based on where I was going, etc.

Thing is, I'm still running into the problem of my machine ignoring the R-variable in the program.

This program is actually pretty short, so I'm going to copy/paste the program and subroutine in below:

Main program first:

(C7015-1P.TXT)
(FOR GEORGIA PACIFIC - HALSEY)
(USE 1" COBALT END MILL @12,500RPM/150IPM)
G90 G80 G40 G10
G90 G1 X240.525 F300
G90 G1 Y63.63
G53.1
M1
G90 G1 Z.25 F21
G90 G1 X1 Y-2.841
G90 G1 Z-.375 F150
G90 G1 X-1.105 Y-2.470
G90 G1 Z-.6
G90 G1 X-4.588 Y-1.855
G90 G1 Z-.375
G90 G1 X-4.739 Y-1.829
G90 G1 Y-2.398
G90 G1 X1 Y-3.4
G90 G1 Z.125
G90 G1 X-5.326 Y-1.725
G90 G1 Z-.125
G90 G17 G75 G3 X-6.273 Y-2.075 R1.0 G1 Z-.6
G90 G1 Z.125
G90 G1 X-5.153 Y-2.315
G90 G1 Z-.125
G90 G17 G75 G3 X-7 Y-2.909 R2.0 G1 Z-.6
G90 G1 Z.125
G90 G1 X-6.273 Y-2.075
M98P013L1 <--I'm only looping once, sample program cutout.
G90 G1 Z-.6 <--all that follows is based on the loop.
G91 G1 X-1.455 Y-1.770
G91 G17 G75 G2 X-1.545 Y0 R1.0 G1 Z.85
G91 G1 X2.273 Y.885
G90 G1 Z-.6
G91 G17 G75 G2 X-3 Y0 R2.0 G1 Z.85
G91 G1 X3
G91 G17 G75 G2 X-3 Y0 R2.0 G90 G1 Z-.85
G90 G1 Z.25
G91 G1 X2.273 Y-.885
G91 G17 G75 G3 X-1.545 Y0 R1.0 G1 Z-.85
G91 G1 X-1.455 Y1.770
G90 G17 G75 G3 X-17.674 Y-1.725 R1.0 G1 Z-.125
G90 G1 Z.125 <--I'll have to change X from here on out.
G90 G1 X-16 Y-2.960
G90 G1 Z-.6
G90 G17 G75 G3 X-17.847 Y-2.315 R2.0 G1 Z-.125
G90 G1 Z.125
G90 G1 X-24 Y-2.841
G90 G1 Z-.375
G90 G1 X-21.895 Y-2.470
G90 G1 Z-.6
G90 G1 X-18.412 Y-1.855
G90 G1 Z-.375
G90 G1 X-18.261 Y-1.829
G90 G1 Y-2.388
G90 G1 X-24 Y-3.4
G90 G1 Z2
M2

And the sub-routine:

(013.TXT)
G90 G1 Z-.6
G91 G1 X-1.455 Y-1.770
G91 G17 G75 G2 X-1.545 R1.0 G1 Z.85
G91 G1 X2.273 Y.885
G90 G1 Z-.6
G91 G17 G75 G2 X-3 R2.0 G1 Z.85
G91 G1 X3
G91 G17 G75 G2 X-3 R2.0 G1 Z-.85
G90 G1 Z.25
G91 G1 X2.273 Y-.885
G91 G17 G75 G2 X-1.545 R1.0 G1 Z-.85
G91 G1 X-1.455 Y1.770
G91 G17 G75 G3 X-1.545 R1.0 G1 Z.85
G91 G1 X2.273 Y-.885
G90 G1 Z-.6
G91 G17 G75 G3 X-3 R2.0 G1 Z.85
G91 G1 X3
G91 G17 G75 G3 X-3 R2.0 G1 Z-.85
G90 G1 Z.25
G91 G1 X2.273 Y.885
G91 G17 G75 G3 X-1.545 R1.0 G1 Z-.85
M99



The urge to save humanity is almost always only a false-face for the urge to rule it. -- H.L. Mencken
 
Upvote 0 Downvote
Any ideas as to what, if anything I'm doing wrong?

Oh, and all code prior to the M1 at the beginning of the first program are positioning codes for the part offset.

The urge to save humanity is almost always only a false-face for the urge to rule it. -- H.L. Mencken
 
Upvote 0 Downvote
Some of our machines (including a less than year old Horizontal mill) can only handle “R’s” in a simple 2D path less than 90 degrees. On a G19 on a recent program, our horizontal was taking “short cuts” across the arcs using “R’s”, so everything went back to “J’s” & “K’s” and quadrant programming. A lot more work for us, but simpler for the machine to calculate.
 
Upvote 0 Downvote
On a previous program, though, it worked just fine.

Here's part of it:


(10439C-1.TXT)
(SOURCE DWG. P10439C BY J. GUYTON)
(FOR SMURFIT-STONE - HODGE, LA. PM 4 SERPENTINE)
(5/8" CARBIDE END MILL @ 12,500 RPM)
(DOES FIRST HALF OF PART)
(RUN 10439C-2.TXT AFTER REPOSITIONING)
G90 G80 G40 G10
G90 G1 X240.525 F300
G90 G1 Y63.63
G53.1
M1
G90 G1 Z.25
G90 G1 X1.4348 Y-2.2881
G90 G1 Z-.5
G90 G1 Z-.5
G91 G1 Y.5
G91 G1 X-.5
G91 G1 Y-1
G91 G1 X1
G91 G1 Y1
G91 G1 X-.5
G90 G1 X1.4348 Y-2.2881
G90 G1 X-1.5 Y-2.718
G90 G1 Z-.800
G90 G1 X-8.281 Y-3.706
G90 G1 X-9.457 Y-3.868 Z.8
G90 G1 X-8.281 Y-3.706
G90 G1 X-9.457 Y-3.868 Z-.8
G90 G17 G75 G2 X-11.156 Y-3.991 R20
G90 G17 G75 G2 X-12.344 Y-3.991 R20 G1 Z.8
G90 G1 X-11.156 Y-3.991
G90 G17 G75 G2 X-12.344 Y-3.991 R20 G1 Z-.8
G90 G17 G75 G2 X-15.227 Y-3.695 R20
G90 G1 X-17.165 Y-3.353
G90 G1 X-18.335 Y-3.147 Z.8
G90 G1 X-17.165 Y-3.353
G90 G1 X-18.335 Y-3.147 Z-.8
G90 G1 X-20.273 Y-2.805
G90 G17 G75 G3 X-23.156 Y-2.509 R20
G90 G17 G75 G3 X-24.344 Y-2.509 R20 G1 Z.8
G90 G1 X-23.156 Y-2.509
G90 G17 G75 G3 X-24.344 Y-2.509 R20 G1 Z-.8
G90 G17 G75 G3 X-27.227 Y-2.805 R20
G90 G1 X-29.165 Y-3.147
...

And it continues on in that vein for quite a long while; about 8K of text, to be exact.

Anyway, it appears I'm going to have to go through the tedious process of "I"s and "J"s (as opposed to J and K on your system) and splitting the arc travel in half yet again.

The urge to save humanity is almost always only a false-face for the urge to rule it. -- H.L. Mencken
 
Upvote 0 Downvote
Status
Not open for further replies.

Similar threads

Julio Baptista
  • Locked
  • Question
Hello everyone! I need your help
Replies
0
Views
13
Julio Baptista
Julio Baptista
Hungy_For_Knowledge
  • Locked
  • Question
I am trying to determine the steel alloy used for the major parts of these snowplows. 2
2
Replies
21
Views
22
Son Tung PHAM
Son Tung PHAM
AbdullahE
  • Question
Hi, What is the meaning of the c 3
Replies
6
Views
76
gtaw
gtaw
pancakeglutton
  • Locked
  • Question
Need Introduction to Die Design
Replies
16
Views
17
malzeri83
malzeri83
MF Afif
  • Locked
  • Question
Element deletion on the broken chips during machining
Replies
1
Views
32
Stick.
Stick.
Back
Top