Second pass with different thread depth?
Helps with the Mach3 CNC Threading functionality
Status: Beta
Brought to you by:
stephanbrunker
Menu
▾
▴
I cannot imagine that to be a regular thread. Do you have a specification? In principle, you can do that manually within the output code, the x value is the thread depth. But if you change that value, the result would invalidate the profile for that specific pitch, because pitch and depth are related trough the specification of that thread. Simply spoken: you wouldn't be able to cut outside and inside thread with a normal angled cutter. Theoretically, it would be possible to create a thread with two passes and different depths it you increase the first pass and decrease the second, but then - you have to make up your own specifications and then you'd have the data for the G76 yourself anyway.
It is a standard thread 1/2 UNF 20 TPI, however when cutting I want to be able to cut deep when starting the thead and then change cutting depth when nearer the finish (to get a better thread finish). This also speeds up the thread cutting process.
e.g.
G0 X12.55
G76 X11.4 Z-32.0 Q1 P1.270 J0.06 L45 H0.06 I29 C1.0 B0.01 T0
G0 X11.4
G76 X11.0 Z-32.0 Q2 P1.270 J0.01 L45 H0.025 I29 C2.0 B0.01 T0
Cut at H0.06 depth from 12.55mm to 11.4mm, then next cut at H0.025 from 11.4mm to 11mm
thanks
Last edit: Goatofmendez 2017-11-27
The program displays a list of all the cutting passes. There are two formulas: Sandvik and equal for calculating the pass depth. Equal means that the cross section of the chip remains constant. For sandvik, the formula is slightly different with smaller increments at the beginning and greater at the finish, the "H" value is only the depth of the first cut.
G76 p1.5 r4.925 x3.813 h0.352 i29.5 k5.782 z-10.0 l360 q0
My calculator uses the same formula than the G76 macro to determine the number of passes out of this H-value, so you can see what the G76 macro will do.
There is one feature: If you want the last pass to have a certain depth, that is the "Sizing" value, the b number.
I did a M8 of 30 mm length a few days ago and it springed away a lot, so normally you'd have to add spring passes (that means, increment 0), which in reality cut a little bit anyway and thus make the finish better, too. To smooth it, i used a rotating steel brush ...
Last edit: stephanbrunker 2017-11-27
Quick questio though - how does mach3 know the difference between a parallel thread and a sandvik?
I got the sae code from both options
Equal thread
G21
G77 r XX x9.931 k5.0 z XX
G76 p0.75 r9.931 x8.81 h0.177 i29.5 k6.641 z-15.0 l360 q2
Sandvik thread
G21
G77 r XX x9.931 k5.0 z XX
G76 p0.75 r9.931 x8.81 h0.098 i29.5 k6.641 z-15.0 l360 q2
Its hidden in Mach3: Config - Ports and Pins - Turn options - Infeed Type
Type 0 is equal, Type 1 is sandvik
Threre you can also set the Cut Type (on which side of the tool to cut) - see Mach3Threading.pdf, page 27, this is normally 0: righthanded flank infeed, cutting mostly at the left edge of the tool.
the x,z clearances and the minimum decrement.
these values had to be the same in the calculator options and in Mach3, that the number and depth of the passes calculated are identical. The same is true for the motor acceleration values. It has no grave implications because the generated code is mostly identical, but to keep the calulations the same, the values should be copied from the Mach3 config.
Last edit: stephanbrunker 2017-11-27
Hi, quick question - when installing the .lset (an corrected Turn screenset
1024-2.lset -> install in %Mach3path%/)
Do you rename 1024-2.lset to -> 1024.lset. Or keep it as 1024-2.lset???
Is there any particular way to install or do you just copy it to the folder?
Thanks
Steve
----------------------------------------------------------------------------
When I came here 17 years ago, you all laughed at me. Well, you're not
laughing now, are you!
Nigel Farage MEP - [Addressing the European Parliament June 28th 2016]
From: stephanbrunker [mailto:stephanbrunker@users.sf.net]
Sent: 27 November 2017 19:28
To: [mach3threadinghelper:tickets]
Subject: [mach3threadinghelper:tickets] #5 Second pass with different thread
depth?
Its hidden in Mach3: Config - Ports and Pins - Turn options - Infeed Type
Type 0 is equal, Type 1 is sandvik
Threre you can also set the Cut Type (on which side of the tool to cut) -
see Mach3Threading.pdf, page 27
the x,z clearances and the minimum decrement.
these values had to be the same in the calculator options and in Mach3, that
the number and depth of the passes calculated are identical. The same is
true for the motor acceleration values. It has no grave implications because
the generated code is mostly identical, but to keep the calulations the
same, the values should be copied form the Mach3 config.
[tickets:#5] https://sourceforge.net/p/mach3threadinghelper/tickets/5/
Second pass with different thread depth?
Status: closed
Milestone: 1.0
Created: Mon Nov 27, 2017 01:11 PM UTC by Goatofmendez
Last Updated: Mon Nov 27, 2017 06:36 PM UTC
Owner: nobody
Can you create a thread with a second pass with different thread depth?
Sent from sourceforge.net because you indicated interest in
https://sourceforge.net/p/mach3threadinghelper/tickets/5/
To unsubscribe from further messages, please visit
https://sourceforge.net/auth/subscriptions/
Related
Tickets:
#5Hi, quick question – when installing the .lset (an corrected Turn screenset 1024-2.lset -> install in %Mach3path%/)
Do you rename 1024-2.lset to -> 1024.lset. Or keep it as 1024-2.lset???
Is there any particular way to install or do you just copy it to the folder?
Thanks
Steve
Try to look at the Mach3 main menu: There is a Item: "View" and a subitem "Load screens"