CamBam
News:
 
*
Welcome, Guest. Please login or register.
Did you miss your activation email?
September 25, 2017, 23:22:40 pm


Login with username, password and session length


Pages: [1] 2
  Print  
Author Topic: Some help please: cutting a slot  (Read 61009 times)
Harold
Storm Trooper
***
Offline Offline

Posts: 126


View Profile
« on: December 29, 2013, 14:55:45 pm »

I need guidance please. Some of this I have figured out but there are other parts to the puzzle which are causing me to draw a blank.

My stock is aluminum. It's 4.005" wide by 8.8125 long. Down the entire length and slotting in the exact middle, I want to cut a slot that's .62135" wide by .0125" deep. My cutter is .500" dia. I want to start at one end and culminate at the other. Incremental cuts will be set to .010" so this will take several passes to complete.

I sketched a rectangle to size then drew a single polyline 10.5" in length and centered the line in the middle of the rectangle. Probably the rectangle is totally unnecessary as I will not be using it for tool paths but it helps me to see things more clearly. Because I will be cutting a slot (entire length), I figured the cutter will need to begin and end outside the rectangle thus I gave sufficient clearance (at both ends) for the cutter to make it past the cutter's diameter by making the line 10.5" long. I SELECTED the center line>RIGHT CLICK>EDIT>OPEN OFFSET>POLYLINE OFFSET and set the numerical value at 0.1. I don't know why I did this, what affect it will have, and I don't know if I did the right thing so please edify me.

I selected PROFILE and began filling in my machining options at the left of my monitor.

Under STYLE, I don't know what to select. Naturally not engrave. So what should I select under STYLE even if this selection plays no part in the actual machining operation?

Clearance, Incremental Depth and Target depth populated.

Cut Feed Rate = 5 and Plunge Feed Rate =5. If you think this is too fast or too slow then please tell me. My spindle Speed is 3740 RPM. If this is too fast then please tell me.

I left Max Crossover Distance and Step Over as .01 and I don't know about this.

Tool Diameter and Tool Profile was populated.

More help is needed here: My cutter is .5" dia but I need the slot to be 0.62135". What do I need to do in order to make the slot 0.62135" wide?

Finally, what do I do to tell the program to start at an end rather than starting in the middle of the work piece?

Harold
Logged

For those having fought for it, Freedom has a flavor the protected will never know.
Freedom is only one generation away from extinction.
atwooddon
CNC Jedi
*****
Offline Offline

Posts: 627



View Profile
« Reply #1 on: December 29, 2013, 15:25:37 pm »

It might be simpler to just make your original rectangle you drew longer than the material and use a pocket operation with that rectangle.  No offsets, just simple pocketing using your .5" bit.

Don
Logged
Bob La Londe
CNC Jedi
*****
Offline Offline

Posts: 2896


^ 8.5 pounds on my own hand poured bait.


View Profile WWW
« Reply #2 on: December 29, 2013, 15:44:28 pm »

I would probably do it like this.  Speeds and feeds assume a standard 30 degree 2 flute HSS end mill with an excessive stickout and flood coolant.  With a rigid machine, minimal stickout, & fresh carbide endmill you could probably cut much faster.  4 flute would be even faster, but chip clearing could be an issue.  If you do not have some form of coolant and chip clearing you are just asking for trouble with this type of cut.  

Speeds and feed taken from this page:
http://zero-divide.net/index.php?page=fswizard

I assumed 6061 aluminum for your mystery metal, but 5000 series (mostly marine grade) is more gummy and harder to cut.  7075 is harder, but easier to cut.  6061, 5052, and 7075 are the most common alloys I run across or work with.  

* Slotting.cb (6.35 KB - downloaded 87 times.)
« Last Edit: December 29, 2013, 15:48:36 pm by Bob La Londe » Logged

Getting started on CNC?  In or passing through my area?
If I have the time I'll be glad to show you a little in my shop. 

Some Stuff I Make with CamBam
http://www.CNCMOLDS.com
Harold
Storm Trooper
***
Offline Offline

Posts: 126


View Profile
« Reply #3 on: December 29, 2013, 16:32:16 pm »

Well DUH! Why didn't I think of drawing a rectangle the size of the cut? DUH!!!! Embarrassed Embarrassed

Bob,

Using Profile why did you choose the following:

Velocity Mode = Exact Stop    What does this do?
Mill Direction = Climb     Why did you elect to use Climb? Is this where you do climb cutting on a finishing pass?
Max Crossover Direction = .7    I really don't know what this function does and why did you choose .7?
Step Over = .4   I don't know what this function does and how did you come about using .4
Tool # = 1   I don't understand that at all. Care to elaborate?

Harold
Logged

For those having fought for it, Freedom has a flavor the protected will never know.
Freedom is only one generation away from extinction.
Bob La Londe
CNC Jedi
*****
Offline Offline

Posts: 2896


^ 8.5 pounds on my own hand poured bait.


View Profile WWW
« Reply #4 on: December 29, 2013, 16:52:43 pm »

Well DUH! Why didn't I think of drawing a rectangle the size of the cut? DUH!!!! Embarrassed Embarrassed

Bob,

Using Profile why did you choose the following:

Velocity Mode = Exact Stop    What does this do?

Quote
Exact Stop will give accurate non rounded cuts stopping at each defined point of geometry.  Constant Velocity rounds off the corners to maintain machine speed, and is affected by the acceleration and decelleration rate of your machine and the defined parameters for CV mode.  Exact stop may leave additional tool marks at points where it stops, but in your case those are outside the work piece.  For 90% of what I do Constant velocity is good enough, but I did take the time to define some limits in my control for my mill regarding constant velocity.


Mill Direction = Climb     Why did you elect to use Climb? Is this where you do climb cutting on a finishing pass?

Quote
Yes, I prefer climb cutting on a finish pass if the machine is rigid enough.  It tends to leave a better finish.

Max Crossover Direction = .7    I really don't know what this function does and why did you choose .7?

Quote
That is the maximum distance (percentage of cutter diameter .7=70%) your cutter will move to start the next cut pass.  In the single pass finish profile cut it has no affect.  In the pocketing operation it keeps the cutter from retracting before it makes the next pass.

Step Over = .4   I don't know what this function does and how did you come about using .4

Quote
It is the default and has no affect in the profile MOP if a cut width is not defined.  If a cut width is defined it is the percentage of cutter diameter that the cutter would step over from the starting pass until it reaches the finish pass.

Tool # = 1   I don't understand that at all. Care to elaborate?

Quote
If your machine is setup to use tool changes (even if its just to stop and move to a convenient location for manually changing the cutter) this will make sure it starts with a tool change in the code.  If the next MOP is the same tool number it will not insert another tool change.  If its different it will.  If your machine is not setup to do anythign with a tool change it will just start cutting at the beginning and ignore further tool changes.  

Harold

I would also note that a .01 in stepover is not .01".  It is 1% of cutter diameter, which is .005" of a .5" cutter.  If you want an increment of .01" set your stepover to .02.  I seem to recall I put .005 in the stepover in the pocket by mistake.  Oops.  I did do the speed and feed calculations based on a stepover of .01". 


Logged

Getting started on CNC?  In or passing through my area?
If I have the time I'll be glad to show you a little in my shop. 

Some Stuff I Make with CamBam
http://www.CNCMOLDS.com
Harold
Storm Trooper
***
Offline Offline

Posts: 126


View Profile
« Reply #5 on: December 29, 2013, 17:12:55 pm »

Thanks to Don and Bob for replying. Much appreciated!

Harold
Logged

For those having fought for it, Freedom has a flavor the protected will never know.
Freedom is only one generation away from extinction.
atwooddon
CNC Jedi
*****
Offline Offline

Posts: 627



View Profile
« Reply #6 on: December 29, 2013, 18:42:22 pm »

Well DUH! Why didn't I think of drawing a rectangle the size of the cut? DUH!!!! Embarrassed Embarrassed

Sometimes the easiest/obvious solution is hard to visualize.  We get trapped into visualizing a part a certain way and get locked into that solution.  I have certainly done that plenty of times.  ;-)

Don
Logged
kvom
CNC Jedi
*****
Offline Offline

Posts: 1383


View Profile
« Reply #7 on: December 29, 2013, 21:17:36 pm »

Here's the way I cut slots like this.  Two parallel polylines defining the sides of the slot, with their lengths being longer than the slot by enough to clear the stock on either end.  The tool cuts full width up one side, crosses over, and cuts down the other side.  Repeat for each depth increment.  To get both cuts inside the slot you may need to reverse the direction of one of the lines.  Attached file shows the technique

* Untitled.cb (4.15 KB - downloaded 83 times.)
Logged
Harold
Storm Trooper
***
Offline Offline

Posts: 126


View Profile
« Reply #8 on: December 30, 2013, 14:15:53 pm »

Bob,

I have the part mounted on the table, have found center, and have moved the table so that the .500" cutter is *VERY CLOSE* (~.002") to touching the end of the work piece (which is where I want to begin the cut).

Because I am just getting familiar with this mill, I prefer at this time, to make multiple passes when attempting the slot rather than completing the cut in one single pass. The part I am about to cut is an important part and I don't want to mess this up. Because I am making multiple passes, I am concerned about the Max Crossover Distance you have suggested in the above reply (.7). You stated in your reply, "In the single pass finish profile cut it has no affect". Since this will not be a single pass cut then how will this affect accuracy if left at .7? Should I be using a different number because this will be a multiple pass cut?

I do not have "Tool Change" on my machine. I assume I will need to remove Tool #1 from your program??

I do not have coolant thus coolant must be applied manually. I assume I need to change this as well??

I would have thought that 40 is a terribly high Feed Rate and especially so if cutting .125" deep. My spindle is turning at 3740 RPM. I just want to be absolutely certain before I proceed.

PS: Bob, it just occurred to me that you set the cutter to begin at the end of the piece as I wished. This would mean that I need to position my cutter in the middle of the work piece (X0, Y0) and then the program will tell the table to move to the end by "x inches". If I place my cutter at the end, as I currently have it positioned, then I assume the table will move an additional 4" away from the work piece. Right?Huh?

Harold


 
« Last Edit: December 30, 2013, 14:43:27 pm by Harold » Logged

For those having fought for it, Freedom has a flavor the protected will never know.
Freedom is only one generation away from extinction.
Bob La Londe
CNC Jedi
*****
Offline Offline

Posts: 2896


^ 8.5 pounds on my own hand poured bait.


View Profile WWW
« Reply #9 on: December 30, 2013, 15:34:12 pm »

I need to know more about the cutter and the machine to know if the cut would be ok.  

Cutter
Carbide?  HSS?  Coating? Stickout?  New & Sharp?  Flutes? Helix Angle?  I prefer uncoated carbide for aluminum cutting, but have on occassion gotten good cuts with HSS as well.  

Machine
Rigidity?  (Heavy Mill, Light Mill, Baby Mill, Router, Noodley wood frame router.)  Horsepower?  Feed Range?  RPM Range?

I would tackle this job in totally different ways on my Hurco Mill, Taig Mini Mill, and Chinese Gantry Router.  

If you reduce feed rate you improve the cut quality, but it will also reduce tool life.  We also don't know what alloy you are cutting which could affect the numbers.  With aluminum cutting coolant and lubricant are very important.  Especially when slotting.  If you do not have the ability to run flood coolant then you might be able to do it by lubricating the work piece with a few drops of a good cutting fluid like Tap Magic (for all metals) and rubbing it on the entire area to be cut with a finger tip.  Then when cutting stand there with an air hose and a blower nozzle to keep the chips gentley blown clear of the work area.  Low pressure is fine.  You need to keep chips out of the path of the cutter, but you don't need to blast them into the mechanicals of your machine.  

I have been told kerosene or diesel fuel make a fair lube for cuttiing aluminum in a pinch.  I have used WD40, and transmission fluid.  I actually had my Taig setup to use flood transmission fluid at one time, but I have gotten tired of the smell of burnt tranny fluid in my shop.  Now it has a spray mister attached to the spindle,  I have it set to run fairly wet.  I am using Kool Mist 77 and distilled water in it now, but on Lloyds reccomendation I am going to try TRIM when I run out.  

You can reduce the depth increment if you like.  No need to cut any faster if you do.  

.7 means that the cutter will stay engaged in the work piece and not retract between each step over as it cuts the slot.  It would make no difference at all unless you changed it to less than the stepover in this simple cut.  It can be important if you had two separate pockets that were less than 70% of cutter distance apart borh being cut by the same MOP or if you were cutting an irregularly shaped pocket, but should make no difference in this case unless for some reason you wanted to retract the cutter on every pass from side to side  Then you would set it to less than the stepover.  If you notice in my exmple I suggested a rough clearance which leaves some material behind to be cleaning up in the profile MOP that runs after.  

No reason to remove the tool number.  There is no reason to write bad code just because your machine doesn't curently use it.  Get in good habits.  

YOU WILL DESTROY SOME CUTTERS AND SOME WORK PIECES.  

If this is such an important piece then make a similar test cut on a piece of scrap.  Then run the complete code you come up with in the air to make sure it cuts where you think it will.  (Zero well above the table)  Maybe test it on a piece of something easier to cut that has been roughed to the size and shape of your actual work piece.  

I have no idea if my cut will work on YOUR machine or not.  You are the best person to determine that.  It was not my intent to do the job for you, and then guarantee it.  I break cutters and destroy work pieces all the time.  Its frustrating as hell, but its part of learning how to do this stuff.  I just wanted to show you one technique for cutting a slot that is less aggressive than just ploughing through the work piece at 100% engagement.  The stepover speed needs to be calculated at 100% engagement. 

At the risk of sounding rude, there is a not so fine line between helping you learn it and doing it for you.  I used to tutor in college, and I am well aware of the the line.  LOL.  

« Last Edit: December 30, 2013, 15:52:03 pm by Bob La Londe » Logged

Getting started on CNC?  In or passing through my area?
If I have the time I'll be glad to show you a little in my shop. 

Some Stuff I Make with CamBam
http://www.CNCMOLDS.com
Bob La Londe
CNC Jedi
*****
Offline Offline

Posts: 2896


^ 8.5 pounds on my own hand poured bait.


View Profile WWW
« Reply #10 on: December 30, 2013, 15:53:42 pm »

I modified the previous post and added quite a bit to it to try and help you through this cut after I first typed it, so you may want to re-read it if you read it before I posted the modifications.  

I need to know more about the cutter and the machine to know if the cut would be ok.  

Cutter
Carbide?  HSS?  Coating? Stickout?  New & Sharp?  Flutes? Helix Angle?  I prefer uncoated carbide for aluminum cutting, but have on occassion gotten good cuts with HSS as well.  

Machine
Rigidity?  (Heavy Mill, Light Mill, Baby Mill, Router, Noodley wood frame router.)  Horsepower?  Feed Range?  RPM Range?

I would tackle this job in totally different ways on my Hurco Mill, Taig Mini Mill, and Chinese Gantry Router.  

If you reduce feed rate you improve the cut quality, but it will also reduce tool life.  We also don't know what alloy you are cutting which could affect the numbers.  With aluminum cutting coolant and lubricant are very important.  Especially when slotting.  If you do not have the ability to run flood coolant then you might be able to do it by lubricating the work piece with a few drops of a good cutting fluid like Tap Magic (for all metals) and rubbing it on the entire area to be cut with a finger tip.  Then when cutting stand there with an air hose and a blower nozzle to keep the chips gentley blown clear of the work area.  Low pressure is fine.  You need to keep chips out of the path of the cutter, but you don't need to blast them into the mechanicals of your machine.  

I have been told kerosene or diesel fuel make a fair lube for cuttiing aluminum in a pinch.  I have used WD40, and transmission fluid.  I actually had my Taig setup to use flood transmission fluid at one time, but I have gotten tired of the smell of burnt tranny fluid in my shop.  Now it has a spray mister attached to the spindle,  I have it set to run fairly wet.  I am using Kool Mist 77 and distilled water in it now, but on Lloyds reccomendation I am going to try TRIM when I run out.  

You can reduce the depth increment if you like.  No need to cut any faster if you do.  

.7 means that the cutter will stay engaged in the work piece and not retract between each step over as it cuts the slot.  It would make no difference at all unless you changed it to less than the stepover in this simple cut.  It can be important if you had two separate pockets that were less than 70% of cutter distance apart borh being cut by the same MOP or if you were cutting an irregularly shaped pocket, but should make no difference in this case unless for some reason you wanted to retract the cutter on every pass from side to side  Then you would set it to less than the stepover.  If you notice in my exmple I suggested a rough clearance which leaves some material behind to be cleaning up in the profile MOP that runs after.  

No reason to remove the tool number.  There is no reason to write bad code just because your machine doesn't curently use it.  Get in good habits.  

YOU WILL DESTROY SOME CUTTERS AND SOME WORK PIECES.  

If this is such an important piece then make a similar test cut on a piece of scrap.  Then run the complete code you come up with in the air to make sure it cuts where you think it will.  (Zero well above the table)  Maybe test it on a piece of something easier to cut that has been roughed to the size and shape of your actual work piece.  

I have no idea if my cut will work on YOUR machine or not.  You are the best person to determine that.  It was not my intent to do the job for you, and then guarantee it.  I break cutters and destroy work pieces all the time.  Its frustrating as hell, but its part of learning how to do this stuff.  I just wanted to show you one technique for cutting a slot that is less aggressive than just ploughing through the work piece at 100% engagement.  The stepover speed needs to be calculated at 100% engagement.  

At the risk of sounding rude, there is a not so fine line between helping you learn it and doing it for you.  I used to tutor in college, and I am well aware of the the line.  LOL.  

Now, go out into your shop and break some cutters. 
« Last Edit: December 30, 2013, 16:28:23 pm by Bob La Londe » Logged

Getting started on CNC?  In or passing through my area?
If I have the time I'll be glad to show you a little in my shop. 

Some Stuff I Make with CamBam
http://www.CNCMOLDS.com
Harold
Storm Trooper
***
Offline Offline

Posts: 126


View Profile
« Reply #11 on: December 30, 2013, 16:35:29 pm »

Bob, I have modified your program. Actually, I re-drew the entire piece for the experience but did used your Crossover number and lowered the feed rate. I even considered running the machine at 1200 RPM.

Bridge Port Knee style 10 X 54 table.

Spindle Range 0 through 5200 RPM

New Carbide .500 cutter specific for aluminum long helix; uncoated, 2 flute ordinary end cutting end mill

Aluminum 6061

Tap Magic is coolant

While waiting for your response, I ran my program in air. All seemed to go well. I'm only concerned that I get as much accuracy as possible. I didn't want the program to cut 70% beyond my prescribed parameters. This was my major concern.

My discipline does not lie in the art of Tool & Die, rather, I am a Maxillofacial Surgeon. Until 22 AUG 13, I rebuilt the faces of our young soldiers having suffered ballistic wound. My canvas is human flesh. I retired form the military in August. My humble machine shop is a means of escape from the horrors of war. I am trying my best to learn machining. I have the capacity to learn ..... and I will learn ..... but I must first crawl before I walk. Please bear with me.

Harold 

Logged

For those having fought for it, Freedom has a flavor the protected will never know.
Freedom is only one generation away from extinction.
Bob La Londe
CNC Jedi
*****
Offline Offline

Posts: 2896


^ 8.5 pounds on my own hand poured bait.


View Profile WWW
« Reply #12 on: December 30, 2013, 17:48:17 pm »

It will NOT go 70% beyond the geometry of your pocket.  It uses the .7 crossover as a percentage of the cutter diameter to determine whether or not to pick up the cutter before moving over to the next primary cut pass. 

ie: 

Plunge
Make Cut
--Is next start point <> 70% of cutter diameter away from current location. 
---- If > 70% then retract cutter, and rapid to next start point. 
---- if < 70% then move directly to next path. 

It really doesn't apply to this application.  Where it applies is if you had irregular shaped geometry where the cutter most go around feaures to get to another part of the cut, or where you have multiple items of geometry that are closer together than the cross over distance. 

Sometimes you do want the cutter to retract on every pass.  Sometimes when doing scanline method (horizontal or vertical) 3D molds I will set the crossover at less than the stepover to force it to retract the cutter on every pass rather than rub and cut on the cavity wall. 

I suspect your machine could cut at the speeds and feeds I suggested, but if you like wait until this evening.  I will be cutting a part with similar feeds later today, and I'll be glad to post a short video clip. 

Your biggest issue will be chip clearing. 
Logged

Getting started on CNC?  In or passing through my area?
If I have the time I'll be glad to show you a little in my shop. 

Some Stuff I Make with CamBam
http://www.CNCMOLDS.com
Bob La Londe
CNC Jedi
*****
Offline Offline

Posts: 2896


^ 8.5 pounds on my own hand poured bait.


View Profile WWW
« Reply #13 on: December 30, 2013, 23:10:31 pm »

http://www.youtube.com/watch?v=ipn8-yA-v3w
Logged

Getting started on CNC?  In or passing through my area?
If I have the time I'll be glad to show you a little in my shop. 

Some Stuff I Make with CamBam
http://www.CNCMOLDS.com
Harold
Storm Trooper
***
Offline Offline

Posts: 126


View Profile
« Reply #14 on: December 31, 2013, 11:21:27 am »

Bob,

I've watched your video and that's interesting. Did I see the head angled, as to say rather than a vertical Z, the Z was inclined toward the operator?

I ran the slotting program and with but only a few minor corrections it produced a very clean, accurate slot. Swarf accumulation was never an issue. Light lubrication with negative pressure ensured a constantly clean work area void of "cuttings".

Harold
Logged

For those having fought for it, Freedom has a flavor the protected will never know.
Freedom is only one generation away from extinction.
Pages: [1] 2
  Print  
 
Jump to:  

Powered by MySQL Powered by PHP Powered by SMF 1.1.19 | SMF © 2013, Simple Machines

Valid XHTML 1.0! Valid CSS! Dilber MC Theme by HarzeM
Page created in 0.159 seconds with 18 queries.

Copyright © 2008 HexRay Ltd. | Sitemap