Art,
I've taken some screen shots in hopes of clearing up ?'s. Yes there does appear to be two issues as you have stated. I went into the tool box and changed the stepover to .003" left the depth of cut at .005, I am using a carbide .016" two flute end mill I don't recall of the top of my head what the depth of cut was but set that as .048". Previously I had gotten the root wall pass and the tangental pass with the origin in the middle of the tooth not the gap between. The first shot is the home screen before clicking on the move to fourth axis button. I then did the screen shot after sending it to 4th axis and before the message disappeared. I then added the rooting (which didn't tell me it was to many passes) and the third shot is that one. I hope that this gives more information than I could impart by typing :-\.
Today the rooting operation not only works right but in the right location as well.
I am on vacation this week so I will try to respond quicker than if I was working till 4pm.
Artk
Cutter to large?
Re: Cutter to large?
:)
Two photos for you on your job. One is with no clearance set. Clearance tells the tool to keep away from the
actual gear by a set amount. Notice when set to zero, the tangental run is in the center of the tooth. This gear is SOO
small however, that the clearance of .030 taken form your snapshot, as compared to the tool size of .016, tells it
to stay 2 diameters away from the wall, this moves the path to a point just about center in the tooth.
Set Clearance to 0, and your problem should go away. Sorry it took me awhile to diagnose this, I dont
often deal with such small gears so didnt notice the offset setting used.
Thx
Art
- Attachments
-
-
Re: Cutter to large?
Art,
That did the trick. I hadn't noticed that setting, when should I use something in that setting? When I have a larger gear and want a finish pass? Thanks for your help! when I get home I'll try to cut it.
Artk
That did the trick. I hadn't noticed that setting, when should I use something in that setting? When I have a larger gear and want a finish pass? Thanks for your help! when I get home I'll try to cut it.
Artk
Re: Cutter to large?
Art:
Yes, if you do a pass in any technique with a roughing tool, its there to keep the tool away from the walls, OR to make a
gear with slightly wider teeth. :)
ARt
Yes, if you do a pass in any technique with a roughing tool, its there to keep the tool away from the walls, OR to make a
gear with slightly wider teeth. :)
ARt
Re: Cutter to large?
Art,
I have finally set up the gear in the mill, but get an error message that the mill can't move with a zero feed rate. In the toolbox I have the tool set as #6, .016 end mill, .4inch/minute feed rate. I don't know if its related but when I try to post gcode to my flash drive I can't save it as a title*.tap but rather I must delete the * and save as title .tap. How do I open in an editor? I use Sprutcam 2007 is there any way to save it to work on it in the editor there?
ArtK
I have finally set up the gear in the mill, but get an error message that the mill can't move with a zero feed rate. In the toolbox I have the tool set as #6, .016 end mill, .4inch/minute feed rate. I don't know if its related but when I try to post gcode to my flash drive I can't save it as a title*.tap but rather I must delete the * and save as title .tap. How do I open in an editor? I use Sprutcam 2007 is there any way to save it to work on it in the editor there?
ArtK
Re: Cutter to large?
Art:
You must get rid of the * , its not a legal character for a file name, it sounds like your file didnt get
a feedrate word. Did you have a number in the Feedrate DRO? If your using Mach3, enter a feedrate in the DRO or just add a F.4 at the start of the file and the file will work anyway. When the program saves the file , filename.tap or whatever, just ask sprut cam to load it, its just a text file, it should load fine.. Ill check to make sure Im putting out the FWord properly... :)
Art
You must get rid of the * , its not a legal character for a file name, it sounds like your file didnt get
a feedrate word. Did you have a number in the Feedrate DRO? If your using Mach3, enter a feedrate in the DRO or just add a F.4 at the start of the file and the file will work anyway. When the program saves the file , filename.tap or whatever, just ask sprut cam to load it, its just a text file, it should load fine.. Ill check to make sure Im putting out the FWord properly... :)
Art
Re: Cutter to large?
Art,
I can't edit the gcode file once it is loaded into Mach 3. If I recall the feed rate was at F4.0 at the time. Is there some reason that the F.4 feed rate that is set in the tool table isn't accepted in the gcode? Or do I have something set wrong?
Art K
I can't edit the gcode file once it is loaded into Mach 3. If I recall the feed rate was at F4.0 at the time. Is there some reason that the F.4 feed rate that is set in the tool table isn't accepted in the gcode? Or do I have something set wrong?
Art K
Re: Cutter to large?
Art:
Theres an edit button in Mach3 that will open the editor.. you should be able to edit it
from there. The Feedrate should have been put in the file, but there is a feedrate box
that overrides the tool value, so if the feedrate box has zero in it on the screen, ( top
of the screen when in 4th axis..right of tool selection, then it may not put the value in
the file. OR.. theres a bug I havent heard of. Either way, no big deal, you should just be able
to enter a feedrate manually in mach3, or hit the edit button an change it in the file..
Art
Theres an edit button in Mach3 that will open the editor.. you should be able to edit it
from there. The Feedrate should have been put in the file, but there is a feedrate box
that overrides the tool value, so if the feedrate box has zero in it on the screen, ( top
of the screen when in 4th axis..right of tool selection, then it may not put the value in
the file. OR.. theres a bug I havent heard of. Either way, no big deal, you should just be able
to enter a feedrate manually in mach3, or hit the edit button an change it in the file..
Art
Re: Cutter to large?
Art,
I tried (after the Packer game of course) what you suggested first, it still won't move if the feed rate box says F.4 and the gcode says F0. Then I discovered you don't edit the gcode you "change gcode". Then it was a simple matter of changing F0 to F.4 528 times, 11 times for each tooth on the gear. Next time I'll load Mach3 on my laptop so I can at least sit while I do it. I'd like to know why, when the feed rate is set for the tool in the tool box and I can see that F.4 in the tool column, does it select F0? It was a PITA to stand there and change each one by hand when it should have been set already. Is it just that it couldn't accept that someone would use F.4 to cut steel?
Art K
I tried (after the Packer game of course) what you suggested first, it still won't move if the feed rate box says F.4 and the gcode says F0. Then I discovered you don't edit the gcode you "change gcode". Then it was a simple matter of changing F0 to F.4 528 times, 11 times for each tooth on the gear. Next time I'll load Mach3 on my laptop so I can at least sit while I do it. I'd like to know why, when the feed rate is set for the tool in the tool box and I can see that F.4 in the tool column, does it select F0? It was a PITA to stand there and change each one by hand when it should have been set already. Is it just that it couldn't accept that someone would use F.4 to cut steel?
Art K
Re: Cutter to large?
Art:
Wow, 528 times, yeah, that'd be a pain. I tend to use find/replace if that happens,
try that and I think youll find it easier..
Now,, as to WHY it happened, Im not sure. Its true thye tool has a default feedrate attached
to it, but the more important numbers are two on the screen, plunge, and feedrate. One will
apply on downward moves, the other in non Z moves.
Now there is also a post processor, labeled "default mill" which specifies how many decimals to use,
mine is set ( and is default in download) to 1 decimal point, which should have served you well,
when I try what you describe, I get a file with ( heres a snippet)
M6 T1
G43H1
M3 S1750
G0 X6.600 Y-0.308 Z0.500 A3.322
G1 Z-2.902 250.0
G1 X-6.600 F0.4
G1 Y-3.803 Z-2.872 A20.103
G1 X6.600
G1 Y-5.029
As you can see, my feed says .4 . Heres what I suggest, when you post, there is a
small checkbox labeled, "Show in editor", this will open the freshly creatd file when you post,
so report that, and look in the editor, if the Feedrate is zero, look at the feedrate and plunge DRO's,
is either of them set to zero? ( I suspect your plunge is zero wince you had so many of them..
Let me know what you find, I cant find any error per say, but I can see if that plunge box is zero
where youd get a lot of F0's inthe file.. Ill add a fix for that in fact so zero is just not allowed..
Art
Wow, 528 times, yeah, that'd be a pain. I tend to use find/replace if that happens,
try that and I think youll find it easier..
Now,, as to WHY it happened, Im not sure. Its true thye tool has a default feedrate attached
to it, but the more important numbers are two on the screen, plunge, and feedrate. One will
apply on downward moves, the other in non Z moves.
Now there is also a post processor, labeled "default mill" which specifies how many decimals to use,
mine is set ( and is default in download) to 1 decimal point, which should have served you well,
when I try what you describe, I get a file with ( heres a snippet)
M6 T1
G43H1
M3 S1750
G0 X6.600 Y-0.308 Z0.500 A3.322
G1 Z-2.902 250.0
G1 X-6.600 F0.4
G1 Y-3.803 Z-2.872 A20.103
G1 X6.600
G1 Y-5.029
As you can see, my feed says .4 . Heres what I suggest, when you post, there is a
small checkbox labeled, "Show in editor", this will open the freshly creatd file when you post,
so report that, and look in the editor, if the Feedrate is zero, look at the feedrate and plunge DRO's,
is either of them set to zero? ( I suspect your plunge is zero wince you had so many of them..
Let me know what you find, I cant find any error per say, but I can see if that plunge box is zero
where youd get a lot of F0's inthe file.. Ill add a fix for that in fact so zero is just not allowed..
Art
Re: Cutter to large?
Art.
Earlier in the week I attempted to cut the gear. Roughed out the first tooth & promptly snapped the cutter on the first pass on the tangental pass of the cutter. Is there some way to keep the cut 20 percent of cutter diameter, that's why I set the step over at .003 of an inch.
Art K
Earlier in the week I attempted to cut the gear. Roughed out the first tooth & promptly snapped the cutter on the first pass on the tangental pass of the cutter. Is there some way to keep the cut 20 percent of cutter diameter, that's why I set the step over at .003 of an inch.
Art K
Re: Cutter to large?
Art:
The step-over should have been exactly as you specified. BUT, again, on the screen under the tool description, is
an override. This is there so you can quickly set any step-over and change it from operation to operation.
Repost the job, but while your doing so, set the stepover override, then uncheck rooting and recheck it. Each time
you uncheck and recheck the rooting box, the job is replanned using the onscreen settings. (Make sure you hit
enter after typing in a new number and before unchecking and rechecking rooting. ).
Do this with larger and smaller numbers and observe the result on the screen of the rooting path. Notice how tight
or loose the passes get together as you enter smaller and larger numbers. Get used to seeing that change so your used to
how it affects all operations. This step-over overrides your tool step-over but only affects the rooting though, for the number
of passes during tangental use the "segments" setting.
Tangental shaving isnt really a stepover, its a matter of dividing the angular change by an appropriate number
of shaving passes. How many you need depends on the gear and the tool, but generally, tangental doesnt take much
off each pass, but in very small tools even that much may be too much, so if you want more passes to reduce
the amount of edge taken each pass, increase the Segments value and uncheck and recheck tangental each time
you do to see the effect. Youll notice the more segments, the finer the passes and the less material removed each pass,
this isnt stepover, but more an angular division.. and so is labeled "Segments".
Take note Art, its not uncommon for a person on their first gear to have their A axis turning wrong
direction, this is because few CNC systems actually have their A axis direction set to any standard.
Make sure, ( run in the air), that the rotary is turning as in the simulation. If it isnt, it will snap
bits every time.. and its not obvious always, Ive had several people cut entire gears in reverse
without knowing why the gear looked so bad..
The rule, is that if you look back in minus direction on the 4th axis parallel axis, and rotate positive (A++),
the gear will rotate CCW.In better words, if your 4th axis chuck is facing X++, and you watch the chuck
from the X++ looking X--, it will rotate CCW if you go A++. This is the standard for rotary axis, but in
my experience almost 50% are set backwards.. youd never notice except in something like tangental
shaving..
Now, as well as segments to lessen how much the tool takes, you can also, in the case of very small
tools, set a clearance and cut the gear with that, and then cut with no clearance, ( or in extreme cases, cut
several times with decreasing clearances..each time less will be taken..
Id suggest you toy with the parameters, and check and uncheck the tangental each time to get a clear
idea of what each does. Its very graphical, and the simulations show what "should" happen, so when you
snap a tool its best to check if all is OK, before just going to finer passes.. Breaking bits in tengental
shaving should be a fairly rare occurance.. except with very small tools, then it can be a complex dance to
get things right..
Art
The step-over should have been exactly as you specified. BUT, again, on the screen under the tool description, is
an override. This is there so you can quickly set any step-over and change it from operation to operation.
Repost the job, but while your doing so, set the stepover override, then uncheck rooting and recheck it. Each time
you uncheck and recheck the rooting box, the job is replanned using the onscreen settings. (Make sure you hit
enter after typing in a new number and before unchecking and rechecking rooting. ).
Do this with larger and smaller numbers and observe the result on the screen of the rooting path. Notice how tight
or loose the passes get together as you enter smaller and larger numbers. Get used to seeing that change so your used to
how it affects all operations. This step-over overrides your tool step-over but only affects the rooting though, for the number
of passes during tangental use the "segments" setting.
Tangental shaving isnt really a stepover, its a matter of dividing the angular change by an appropriate number
of shaving passes. How many you need depends on the gear and the tool, but generally, tangental doesnt take much
off each pass, but in very small tools even that much may be too much, so if you want more passes to reduce
the amount of edge taken each pass, increase the Segments value and uncheck and recheck tangental each time
you do to see the effect. Youll notice the more segments, the finer the passes and the less material removed each pass,
this isnt stepover, but more an angular division.. and so is labeled "Segments".
Take note Art, its not uncommon for a person on their first gear to have their A axis turning wrong
direction, this is because few CNC systems actually have their A axis direction set to any standard.
Make sure, ( run in the air), that the rotary is turning as in the simulation. If it isnt, it will snap
bits every time.. and its not obvious always, Ive had several people cut entire gears in reverse
without knowing why the gear looked so bad..
The rule, is that if you look back in minus direction on the 4th axis parallel axis, and rotate positive (A++),
the gear will rotate CCW.In better words, if your 4th axis chuck is facing X++, and you watch the chuck
from the X++ looking X--, it will rotate CCW if you go A++. This is the standard for rotary axis, but in
my experience almost 50% are set backwards.. youd never notice except in something like tangental
shaving..
Now, as well as segments to lessen how much the tool takes, you can also, in the case of very small
tools, set a clearance and cut the gear with that, and then cut with no clearance, ( or in extreme cases, cut
several times with decreasing clearances..each time less will be taken..
Id suggest you toy with the parameters, and check and uncheck the tangental each time to get a clear
idea of what each does. Its very graphical, and the simulations show what "should" happen, so when you
snap a tool its best to check if all is OK, before just going to finer passes.. Breaking bits in tengental
shaving should be a fairly rare occurance.. except with very small tools, then it can be a complex dance to
get things right..
Art
Re: Cutter to large?
Art,
I went out in the shop and fired up the machine and sure enough the A axis was reversed. After spending quite a while on the phone with the tech guys at Tormach I think I have that sorted out. I had to go and reverse the wires on a few drivers cause they were backwards. I have an early Tormach mill and had to install the 4th axis myself. That doesn't explain why all the other drives ran backwards from the pendant though. My machine is early enough that a lot of it was still in the development stage. And they didn't have good records of those original setups. I think I will need to make a new blank for the gear. The lines in the gear that I initially thought were caused by the broken tip of the cutter are actually separate passes of the cutter, probably .040" deep. That little thing was tougher than I gave it credit for. I already know it will do the roughing pass I might forward it to the tangental portion and see how it looks there.
Art K
I went out in the shop and fired up the machine and sure enough the A axis was reversed. After spending quite a while on the phone with the tech guys at Tormach I think I have that sorted out. I had to go and reverse the wires on a few drivers cause they were backwards. I have an early Tormach mill and had to install the 4th axis myself. That doesn't explain why all the other drives ran backwards from the pendant though. My machine is early enough that a lot of it was still in the development stage. And they didn't have good records of those original setups. I think I will need to make a new blank for the gear. The lines in the gear that I initially thought were caused by the broken tip of the cutter are actually separate passes of the cutter, probably .040" deep. That little thing was tougher than I gave it credit for. I already know it will do the roughing pass I might forward it to the tangental portion and see how it looks there.
Art K
Re: Cutter to large?
Hi Art,
Thats good news anyway. As I said, its not unusual at all for a machine to rotate A in reverse, most dont know
the spec for it and its rare to use a 4th axis in this way. The code form the gear cutter has proven to be pretty bulletproof
over the last while, Id say the only real reports of trouble have been the rotation direction, as its not very intuitive
when its wrong. Seems right, just snaps tools. and only in tangental phase..lol
Hopefully your now off to the races.. Let us know how your gear looks, I think you'll find each one gets better
as you get used to how it all works..
Art
Thats good news anyway. As I said, its not unusual at all for a machine to rotate A in reverse, most dont know
the spec for it and its rare to use a 4th axis in this way. The code form the gear cutter has proven to be pretty bulletproof
over the last while, Id say the only real reports of trouble have been the rotation direction, as its not very intuitive
when its wrong. Seems right, just snaps tools. and only in tangental phase..lol
Hopefully your now off to the races.. Let us know how your gear looks, I think you'll find each one gets better
as you get used to how it all works..
Art
Re: Cutter to large?
ArtK get notepad++ it has find and replace function with it, the 528 changes you made would of been a snap find F0 replace with F.4
Who is online
Users browsing this forum: No registered users and 5 guests