Hello Guest it is December 12, 2019, 10:42:40 AM

Author Topic: Free G76 Macro Helping program for Mach3 Turn  (Read 27869 times)

0 Members and 1 Guest are viewing this topic.

Offline RICH

*
  • *
  •  7,377 7,377
    • View Profile
Re: Free G76 Macro Helping program for Mach3 Turn
« Reply #20 on: January 25, 2016, 11:13:35 AM »
COMMENTS:

1. Would be nice if the following fixed sizes were included in the
the Thread Spec:
   #0 to #12 UNF
   #1 to #12 UNC

   Also American National Standard Taper Pipe Thread
   1/16 to 2 NPT.

2. If leaving the range of the thread tables......
   What kind of unpredictablity may happen?

3. What if one wants to cut a Class 3A thread?

4. Here is something to consider, that's different / not found in most of these
    kinds of helpers and works nicely if you have an accurate lathe:
    Use Cut type 1, reduce the depth of cut, and you can end up with a nice Acme thread
    that can be done on a less powerfull lathe with a sharp v tool!

5. I do have a concern, I am wondering if fooling with the macro or whatever is going to screw up the threading
    .........as the threading cycle was designed when fixed. Spindle slow down, averaging, and sampling may be affected.
    Need to re-read  your notes more than just a quick read. Maybe Newfangled didn't want your help for an undisclosed reason.

Just some feedback,
RICH
 
Re: Free G76 Macro Helping program for Mach3 Turn
« Reply #21 on: January 26, 2016, 04:29:52 AM »
Hello,

adding NPT, Class3A and the small UNF/UNC is simple. Because I'm from the millmeters and metric following, I simply don't know which of these - for me exotic - threads are mostly used. I've a table with #1 - #6, #8, #10 and #12, they have fixed sizes in fractions of an inch and not something like  the x/2^n for the other imperial threads? Does this subgroup has a special name, because I've to make a new entry for them in the drop-down list.

And "if you leave the tables": Basically, what I do for the tolerances is converting the tables to third-order equations. For the range of the tables, I've minmized the difference between the equations and the tables to less than 1/100 mm. But I don't know how the equations behave outside. For 10% more, it should be no real difference, for a diameter 10 times the biggest one in the tables, the values are surely wrong. I did it that way to have the ability to generate threads that aren't in the tables. If you enter 216/1000 inch with 24 TPI for the #12 UNC, you get the right values, I included that range.

Do you have any data for the Acme thread?

Basically, at Newfangled they said that they don't want to change anything at Mach3 anymore, 066 is definitively the last release forever, more or less end-of-life'd it.  And for Mach4, it's not a community project but that of a professional software company which simply does all the work itself and not revealing a scrap of the source code to any outsiders - or have any contributions from them. And about fooling with the macro: Basically, it wasn't programmed very clean. The macro only generates a code of G0, G1 and for the tread G32 moves and that you can change how you want. You can check that out with activating test mode, in this mode it outputs the generated code in a file. The only secret is the special threading mode, entered with two G32 concatunated to chain the retraction move to the previous G32. And that I've tested thoroughly. The threading itself as in the G32 move cannot be tampered with, that's completely internal.
« Last Edit: January 26, 2016, 04:33:38 AM by stephanbrunker »

Offline RICH

*
  • *
  •  7,377 7,377
    • View Profile
Re: Free G76 Macro Helping program for Mach3 Turn
« Reply #22 on: January 26, 2016, 06:48:02 AM »
Stephan,

Can you send me a personal message with your email address. I have some reference material / standards, but, I can't post them for the general public.

RICH



Offline RICH

*
  • *
  •  7,377 7,377
    • View Profile
Re: Free G76 Macro Helping program for Mach3 Turn
« Reply #23 on: January 26, 2016, 09:17:20 AM »
No special name for the #0 to #12. See the attached chart for what belongs to UNC and UNF.
These size threads are used a lot by a lot of folks. Forget about cutting  internal threading for them.
The tolerance on these small sizes are very tight.

Just for info, the tolerance on pitch for Mach threading was based on comparing the pitch over an actual cut length.
There is a chart in the Threading On the Lathe write up (page 26).

I will get you data for the Acme threads and NPT. 

Some practical info on the Acme threads:
- It takes some HP to cut the thread, and a wimpy lathe is not going to do it.
- Most folks will use proper insert ( single or even chasing) and most amateurs will never grind a cutter for it properly.
  ( before someone barks! ) the generated code must assume a properly ground cutter and accurate enough cnc lathe to do the work,
  thus, it's not about the nut goes  on and life is good....enough said.

So what code is generated depends on what method and tool you will use to cut the Acme thread.
Maybe just provide another Tool input / choice for something like: Sharp V  or  Acme Insert.
Just a few thoughts for your consideration.

RICH
Re: Free G76 Macro Helping program for Mach3 Turn
« Reply #24 on: January 26, 2016, 09:55:51 AM »
The table I've found has these threads in it, also NPT/NPTF and NPSM/NPSC. So that is no problem. There I've also the tolerances for the UNC. My code outputs the middle of the tolerance field, so in that case for UNC #12 the flank diameter would be 4.84 mm with a margin of 4/100 mm to each side, thats for class 3A and part of why I left these small ones out. More practiable to use a screwing die. The smallest tool I own for inside threads work from bores of 3 mm upward ...

And for the ACME or the Tr ... trapeze threads:  Perhaps it would be possible to cut a TR with 30° flank angle and a sharp 30° tool, but for that, I'd have to change the M1076.m1s macro on a fundamental basis to cut to the right depth in the first step and then wide it in pitch direction. Possible, but for an clean implementation, the GCode Interpreter of Mach3 has to be changed to add a new variable, and that is - see above - not possible as much as I'd like it to - think of the bugged T-Word. With the right cutter, it is only the depth to respect. So, I think it's going too far. If a change in Mach3 would be possible, I'd do it, but as it now looks, a clean solution is impossible.

Offline RICH

*
  • *
  •  7,377 7,377
    • View Profile
Re: Free G76 Macro Helping program for Mach3 Turn
« Reply #25 on: January 27, 2016, 09:15:14 AM »
Quote
And for the ACME or the Tr ... trapeze threads:  Perhaps it would be possible to cut a TR with 30° flank angle and a sharp 30° tool, but for that, I'd have to change the M1076.m1s macro on a fundamental basis to cut to the right depth in the first step and then wide it in pitch direction. Possible, but for an clean implementation, the GCode Interpreter of Mach3 has to be changed to add a new variable, and that is - see above - not possible as much as I'd like it to - think of the bugged T-Word. With the right cutter, it is only the depth to respect. So, I think it's going too far. If a change in Mach3 would be possible, I'd do it, but as it now looks, a clean solution is impossible.

No problem on not doing the Acme as many folks probably will never use it.
All one needs to do is  use the alternate flank cutting with a sharp V tool but define the proper X end in the Simple Threading Wizard.
The program doesn't know what tool you are actually using and thus it stops the cutting at x end. The tool will just alternately
remove material based on pass depth, doing one side and then the other and stop at Xend. I will add that the cnc lathe needs to be accurate
as it is the equivalent of doing multiple start thread.

I though I had the ASME Standard for ACME thread somewhere but can't find it! Only have ANSI / ASME B1.20.1

Thanks what you doing as I appreciate it,

RICH
Re: Free G76 Macro Helping program for Mach3 Turn
« Reply #26 on: January 27, 2016, 05:27:09 PM »
I'm head first in the threadtables now. I corrected one big bug ( threads in full inches had dia 0) and I'm thinking about the tool radius because - that was also wrong - for some threads it's allowed for the tool tip to be sharp, and for some others, not. For BSW and BSF the inside thread can be sharp, but the outside thread has to be rounded at the bottom, there is a minimum value defined. Now I'm thinking how to realize that. For NPT, the value given is the width of the chamfer and not an radius. So, basically you can have two kinds of tools: some with an radius and some with an chamfer - and the limit calculations are different, of course. And, to get it all together, the trapeze treads are kind of in this too. I've broken some tools, especially thin ones. So, a sharp 30° tool is likely going to break. But you don't need a full set of tools for every trapeze thread if you have some with a chamfer more than half of the width at the bottom of the thread, cut alternating flank and shift the other flank for the missing width of the tool.

Offline RICH

*
  • *
  •  7,377 7,377
    • View Profile
Re: Free G76 Macro Helping program for Mach3 Turn
« Reply #27 on: January 27, 2016, 07:00:06 PM »
Quote
I'm head first in the threadtables now.

May the one above give you patience.

There are so many standards relative to threads and one dosen't know how ill educated they are until you really get into it.
I found hard copy of a few ANSI standards I had. You need to purchase the standards as they are not free from the different organizations.
I know your having fun and learning a lot also.

In the end sometimes "the nut goes on" does have a practical meaning in terms of tolerance. Frankly, I try to do a Class 3 and if it doesn't spec,
well, then I have a class 2. For an NPT, it takes some care in all that one does, since in the end most will be only able to check how many turns it takes to lock up and that the threads all make contact at lockup. What is important from a design perspective is what the thread needs to accomplish, and that ends up having all of these different standards to address the different needs.

Oh, BTW, there no such thing a sharp V tool since every threading tool will have a radius of some value and that needs to be taken into account.
Even if you do grind the tool on a grinding machine it has a silly radius at the point, and if it is say only 0.001" rad that tip radius will break off
in short order.

Just some insights for those following this thread,

Have fun,

RICH


Re: Free G76 Macro Helping program for Mach3 Turn
« Reply #28 on: March 03, 2016, 10:42:56 AM »
Anyone,

When I try the G76 thread helper, I get the following:
G20
G77 r XX x0.6175 k0.0 z XX
G76 p0.0909 r0.6175 x0.4828 h0.0426 i29.5 k0.3525 z-0.5 l360 q0

in MachTurn I use the macros that come with the G76 thread helper when you download and Mach gives me an error at the G77 line.  Does anyone know whats wrong?
Re: Free G76 Macro Helping program for Mach3 Turn
« Reply #29 on: March 03, 2016, 11:14:25 AM »
The G77 (Turning) is to bring the material to the outside diameter of the thread first - in this case 0.6175''. But it cannot know from which chunk of material this is. So, you have to replace the "XX"es for r with your start dia. For example, you can start with a 0.75'' dia and bring it to 0.6175''. The length z should also be greater than the 0.5'' of the thread to avoid a collision with the uncut part. So, put in there your values or if you do it manually, just delete the G77 line. In either case, you have to change your tool between the two lines, because you will use different tools for roughing and thread cutting ;-)

So, a full code may look like this:
Code: [Select]
g18 g21 g40 g90 g94 g80
s350
f40
t0202
g0 x12 z2
m3
#101 = 1.7899
G77 r5 x3.94 k0.0 z-7
g0 z30 x20
m5
t0404
s120
f15
m3
#101 = 1.7899
G76 p0.75 r3.866 x3.297 h0.232 i29.5 k3.141 z-5.875 l540 q0
m5
m30
« Last Edit: March 03, 2016, 11:27:54 AM by stephanbrunker »