Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: Whacko on December 24, 2007, 10:09:29 AM
-
Ok, this is it! MERRY XMAS TO ALL!!!
Whacko on holiday!!!!
-
Ok, this is it! MERRY XMAS TO ALL!!!
Whacko on holiday!!!!
SLACKER!!!!!!!!
:D
-
Ok, this is it! MERRY XMAS TO ALL!!!
Whacko on holiday!!!!
I Gotto slacker, otherwise I might cracka! LOL!
Whacko
SLACKER!!!!!!!!
:D
-
You stopped a bit early - it wasn't even Christmas day :D
-
It's all relative, you know. Space time. The empty space between my ears and the time I take to fill an empty (void)
Happy holidays!
Whacko
-
OK I lied, I'm back! These folks at home are all tanked up, it got boring, so I'm bright eyed and bushy tailed and they are vocally impaired!
Whacko
-
Welcome back Whacko, (you seem bored an anxious to help.)
I've got a question for ya. I'm running Mach3 Turn... Thread cutting with the wizard and hand writing the code.. How can I make the threading tool pull out,(X pos.), and not leave a 60 deg. groove at the end of the thread ? Seems like whatever I do, I can't make it look like I cut it manually. I have double nuts on the ball screw and ZERO backlash but can't make it pull out right.
Thanks Whacko, or anyone else.
RC
I tried rpm from 1300 , 700, and 400.... all the same. Also varied the pull-out angle. No change.
Would like to extend each pass, (Z-) but don't know how...???
-
Old habits die hard. I was a lecturer, seems I still want to lecture! LOL! Can you post one of your nc part programs? Let's have a look.
Whacko
-
SURE !
I gotta run out to the shop and copy it...................................be right back. DON"T GO NOWHERE!
-
Here
-
I'll have to get back to you a bit later, entertaining a sloshed family memeber
Whacko
-
YEAH............I'VE GOT SEVERAL MYSELF. FIRST THINGS FIRST.
-
In the G76 cycle the L word is the one that controls the exit angle, try L90 and a slow speed, 200 RPM, you may be able to go faster but it depends on the speed of your system.
Graham.
-
As mentioned earlier, I tried various L angles. 0,30,45 and 60 deg. with no difference. The manual says L is optional so rather than leaving it out of the line I just put L0 assuming that would be the same as no entry. I'll try L90 tomorrow and slow it down a bit.
I hope I don't have to slow it too much just to get it to pull out right. Everything else is perfect at 700-800 rpm.
Thanks,
RC
-
If you think about what's happening here, you are asking the tool to feed out of the thread in 1/4 of a turn of the thread.
If you are running at 750 RPM that is 12.5 revs per second, that means the tool has to get out of the thread in 0.02 seconds. Not in my life time :o.
That is why it has to run sllloooowwww.
Graham.
-
Ahhhhhhh..........YES. Now that you put it that way, it makes a lot of sense.
That would be asking a bit much at high rpm.
Hopefully, the groove will be acceptable.
Thanks Graham,
RC
-
:)
Graham.
-
Graham,
This is strange to me...when I put in L90, the threading cut started in the opposite direction...towards the tailstock and kept on all the way to the Z+ limit. Entry <90 works OK.
Is this normal ?
Thanks,
RC
-
That's a new one to me, I have asked Art for comments.
Graham.
-
Hi Graham:
The G76 is actually a macro M1076.m1s located in the Mach3 folder. Ill ask Brian to add
that to his list, I suspect the math falls apart at 90 degrees . I suspect the math is falling apart over 89..
Art
-
I added it to my list... I am working on some other code but will have a look as soon as I am done.
Thanks
Brian
-
Thanks Guys,
No hurry on my part, I'm sure you're plenty busy.
The thread as coded is +/-.2" long.
Art is absolutely right ! (I'll bet he gets that a lot.)
L85 works OK,
L88 goes in the wrong direction .5" or so , then reverses and runs toward the spindle about 1" while angling out, then cycle ends normally.
L89 " 1" " 1.5"
Thanks,
RC
-
I have sent a new G76 macro to Brian and Art for there approval, if my code is right this should hopefully fix the problem.
Graham.
-
Which axis is the L angle measured from, X or Z ?
Reason I ask... would L90 typically pull straight out with no chamfer or taper ?
And would L10 cut a long chamfer or taper towards the chuck ? If so, it's from the Z axis...right ?
If it's from the X axis, L10 would pull out nearly straight away and L80 would cut a long chamfer or taper towards the chuck...would it not ?
The way this is now, L80 cuts a longer taper than L30 does. But L100 pulls out angling away from the chuck over the threads.
I realize something is wrong, I'm
just wanting to know how it is intended to work.
Thanks,
RC
-
I think the macro was a bit wrong.
I have recoded it to work like the big machines do it.
So the tool now comes out over a rotation angle set by the L word.
L180 will bring the tool out over .5 of a pitch L270 over .75 of the pitch etc.
Graham.
-
Ahhhh..........angle of ROTATION...never crossed my mind. PERFECT !
That makes more sense.
I assume it will work with a single pulse per rev from the spindle input.
When can I expect it for download ?
Thanks again,
RC
-
I have sent the macro to Brian and Art, as I do not have the authority to post modified versions of there original code they will decide if it gets into the distribution.
Sorry, its all I can do at the moment.
Graham.
-
One other thing weird about thread cutting.
When the cut gets to the point where the tool begins to pull out, the Z axis begins to slow as the X axis retracts the tool.
It appears to be making a G1 move at feed rate from the depth of the cut to the C clearance..which slows Z.
Seems like Z speed, in relation to the spindle index, should not change until the C move is done.
At 400 rpm, L45 deg., the X axis doesn't move more than about 30% of full speed. (+/-)
Hopefully, this will be corrected with the change as well.
Regards,
RC
-
RC:
No, that part sounds normal. The move is a syncronised move at requested feedrate, so as it pulls out, the X ratio is higher so the Z slows down. I dont think anything can be done about that one..
Art
-
Graham,
Macro looks good and will be in the next rev
Thanks for looking at it
Brian
-
Thanks for the reply ART,
You do see what I mean.
It would be best if the actual thread pitch never changed while X pulls back. That would eliminate any grooving at the end of the thread.
Just like when cutting by hand...X out first, then disengage the half nut. Perfect pitch.
If this could be done, rpm could be increased too.
RC
-
Graham,
In Brian's response to you, he said your macro would be in the next rev.
Did he give you a timeframe of when it might be released ?
Being it's approved, can you send it to me in advance ?
I submitted parts to a customer for approval and they were rejected but told them of the changes in progress.
We are anxious to satisfy our customer who is otherwise pleased with the part.
Thanks,
RC
-
Hi:
The macro will be in the next release. But heres an advance copy of th emacro involved..
Art
-
Thank You ART,
I saved it in the Turn Macro folder replacing the orig. 1076 file, is that right ?
I will try it later today .
Thanks again,
RC
BTW....NICE CAT ! Did you train it ?
-
Hi:
Id put it in the C:\mach3 folder. As I recall, thats a special macro which is the same for all profiles,
and resides in the Mach3 folder, not the macros folder..
Art
-
Hello all,
The new macro works quite a bit better. I experimented with L90 through L1440 and it does very well. Results are as expected.
There is only a very slight pause that causes a very slight change in the pitch at the point where the tool begins to pull back.
The Z slows also but not as much as before.
Not perfect.. but much MUCH better.
I don't want to appear picky but this is a delicate part and my customer is the picky one.
Thanks for your help folks,
RC
1 Question: Which is commonly used for thread cutting, Constant Velocity or Exact Stop ? Please explain.
I searched the manual and found no reference to this.
Thanks again.
-
Well at least its better than before. :)
when cutting threads you should always use exact stop mode if cutting into a groove. if you use cv then the thread can become tapered towards the end of the cut due to cv blending corners.
The slight pitch error is probably the reaction time of your machine and the signal processing time of your system.
To get the best results from threading you must allow time for the machine to react, even on fast industrial machines you have to allow acceleration and deceleration times.
Allow 5mm (.200") in front of the thread for acceleration and 2.5 (.100") if possible at the back for deceleration. Also keep the speed down, if the exit looks ragged halve your speed. It is impossible to say what speed to use as every machine is different but start low e.g. 100 rpm and work up.
Using the new macro you could issue a L720 and allow the thread to feed out over 2 pitches thus giving a very smooth and neat exit.
Graham.
-
Thanks for making all of this clear. EXCELLENT explanation. This will go in my notebook, supplement to the M3Turn Manual.
L720 IS where I actually ended up with the best final results.
The customer is more satisfied as well.
Grateful,
RC