Hello Guest it is November 16, 2019, 06:28:30 PM

Author Topic: Simple Threading Wizard Problems HELP  (Read 6492 times)

0 Members and 1 Guest are viewing this topic.

Re: Simple Threading Wizard Problems HELP
« Reply #10 on: September 10, 2009, 10:49:12 PM »
I understand that but I cut external threads all the time no problem. The problem is when cutting internal threads every few cuts it'll do a tapered cut in air, but it doesn't clear the last few threads and chews them up, that's what I asking about, why this is happening and what I can do to stop it or add more clearance when Mach needs to do a test cut.

Offline RICH

*
  • *
  •  7,371 7,371
    • View Profile
Re: Simple Threading Wizard Problems HELP
« Reply #11 on: September 10, 2009, 11:13:04 PM »
When i get my lathe conversion done it will be one of the things i'll check, but until then, don't know what to say.
RICH
Re: Simple Threading Wizard Problems HELP
« Reply #12 on: September 11, 2009, 03:52:53 AM »
No problem, I wonder if I sped up the RPM so there isn't so much friction when doing internal. I notice when doing external I run at 700 RPM and about .01 and .015" per pass and they come out silky smooth. For internal I run 700 RPM and the same .015" per pass and the sides of the threads have patterns where you can see where it's chattering. On my 9x20 HF I have it working perfect but at higher speed I always get chatter from doing ANYTHING internal threads or just cutting, no matter what tool or bit I use, at least on aluminum. So I will try some different things. First slower with smaller cuts and then faster with smaller cuts and see what happens. I think the Gcode that the Simple Threading Wizard puts out is normal Gcode? So even if I wrote a threading program by hand Mach is still doing something on it's own for timing?

Offline Hood

*
  •  25,856 25,856
  • Carnoustie, Scotland
    • View Profile
Re: Simple Threading Wizard Problems HELP
« Reply #13 on: September 11, 2009, 04:23:53 AM »
If you open the m1076.m1s macro in the editor and change the line that says

Test = False

to

Test = True

then Mach will output long code, try that and see if you still get the issues.
 You wont be able to do any other code with threading whilst it is in test mode. The macro is in the main C:\Mach3 directory.
Hood

Offline RICH

*
  • *
  •  7,371 7,371
    • View Profile
Re: Simple Threading Wizard Problems HELP
« Reply #14 on: September 11, 2009, 06:23:02 AM »
What Hood recomended in reply #13, is, the code posted will include all the pass #'s and all the x & z axis moves for a G32 ( instead of G76 code ).  
 
There is no problem with the code ( g76 or g32 ) so don't see any reason to hand code.  Should that xz move happen you will then know what pass it happened at, but, it's kind of random around the 6 th to 12 th ( somewhere in there) if memory is correct. Changing the speed and feed will change the rpm variation you are experiencing.
The problem is not the result of the generated axis moves in the code. So changing the code would be fruitless. The xz axis move you experience has to do with the thread programing as said before.

You can  try changing the settings for  the infeed angle in the wizard. I use 15 degrees for a deeper thread, like 13  to 20 TPI. This way your flank cutting and the motor load is not as great. You can probably reduce the load by 50%
( roughly speaking as i would need to calc the HP differences, and the calcs are rather subjective ).

Mach monitors  each thread cycle and adjusts the mext cycle according to rpm variations.

Try reducing the tool overhang or make it more rigid  to reduce chatter. Of course cutting fluid / speed / depth of cut also come into play when cutting internaly or externaly.

RICH
RICH
« Last Edit: September 11, 2009, 06:24:59 AM by RICH »
Re: Simple Threading Wizard Problems HELP
« Reply #15 on: September 11, 2009, 01:31:43 PM »
Hmmm, now I'm a little confused. Rich are you saying that the problem is with the simple threading wizard and Mach doesn't make those sort of moves on it's own for timing or anything else?

As for tool and coolant, the tool barely sticks out and I always use mist coolant. The chatter is just normal and I know how to get around it.

Offline RICH

*
  • *
  •  7,371 7,371
    • View Profile
Re: Simple Threading Wizard Problems HELP
« Reply #16 on: September 11, 2009, 03:48:38 PM »
No, your confused. There is nothing wrong with the gcode that the wizard generates. The generated gcode just changes the x & z axis locations for each cut of the thread based on what was defined in the wizard. Mach controls execution of the wizard gcode by sending out the appropriate steps and saying when the threading should start and stop and also monitors what is going on while the actual thread is being cut. The combination z & x ( angular ) move you are seeing is part of the Mach / controller.
RICH
Re: Simple Threading Wizard Problems HELP
« Reply #17 on: September 18, 2009, 02:47:15 AM »
OK, so I did some cutting today and I noticed that if there was the slightest drag it would do that taper cutting thing. I set my RPM at 1000 and cutting depth of .01 per pass and the threads came out silky smooth. I still don't understand why if the RPMs drag when cutting that it would start to make a taper cut and gall the threads, seems to be a pretty bad bug. Anyway, I'm fine with it now, I just won't be able to leave it alone while cutting threads for fear of the problem returning.

If anyone can tell me in the Mach Simple Threading Wizard what the relation of Depth of First Pass to Min. Pass Depth in the settings page? If change the Min Pass Depth in the settings page it changes the number of passes the program will make to complete the thread. If that directly controls the number of passes then why on the first page of the wizard does anyone care about the first pass depth?

Offline Hood

*
  •  25,856 25,856
  • Carnoustie, Scotland
    • View Profile
Re: Simple Threading Wizard Problems HELP
« Reply #18 on: September 18, 2009, 03:45:09 AM »
Often you want the first pass to be a greater depth than the rest as there is not so much drag on the first so you can cut deeper and thus overall cycle time is less.
Hood

Offline RICH

*
  • *
  •  7,371 7,371
    • View Profile
Re: Simple Threading Wizard Problems HELP
« Reply #19 on: September 18, 2009, 08:49:48 AM »
Threading is a rather complex and interesting machining operation. There are a lot of factors that
come into play when it is done. Material, spindle speed, cutter geometry, cutting fluid, depth of cut

and also type of threading method to be used all come into play and are interelated to each other.

You can get very techie about it and do calculations to see the affects of different combinations. In

fact over the years, it has been studied in depth and testing conducted to try and put threading

material / metal cutting into some good engineering perspective. The SME ( Society of

Manufacturing Engineers ) has done research and many of the insert manufacturers base their

calculations for diffferent tools to maching parameters on the research. All that stuff is fine, but, it is

still subjective in nature, in the sense that, so many considerations come into play when

calculated. That is not to say that one would not benefit greatly by reviewing the information.

As Hood noted the first cut is usualy deeper and you can save time and minimize the number of

remaining passes. Kind of depends on how you want to work and what works for you. You may

want to take a smaller cut just to see that all is working and you are setting a groove for the tool to

follow. Yet , you may want to take a cut that would give you the same material removal rate as the

of all the remaining cuts as that would give you an indication of what how your machine will behave

when cutting the thread. If too deep and just a radial cut you may take the tip off the cutter.
If the material work hardens then you change what you are doing again. Some soft materials are

just as bad or even worst than harder ones.

That a look at the generated code of the wizard and note how the Z and X values change from one

pass to the next. Then change the infeed angle and compare the Z and X moves to the other infeed

angle setting. 30 or 29 infeed angle is good for very fne threads, yet 15 would be a better value for

harder and deeper threads.

Note that as you increse the RPM the stepper acel rate will increase and a good rule of thumb
is to allow 3 to 5 times the depth of cut for the acceleration to take place ( that requires setting the

tool in the Z+ away from the material ). Idealy you would want max power from motor. If you have
 a punny lathe with a small motor then speed may become important since you want the the rpm

so it won't slow down, but, it's motor and gearing related. You may want to take a look at my post

on converting a lathe in the members docs as i included some graphs and how rpm, stepper torque,
, motor horsepower and feed rate are related.  

Just some practical comments on threading for your consideration,
RICH