add optional p word to set peck distance/count

[rene-dev]

adds optional p word to #1860

[hansu]

Is it intended that this PR includes Chris' commits?

[petterreinholdtsen]

[Rene Hopf]

adds optional p word to #1860/

Nice. Hos is this related to other G-code dialects? Note, If I am to believe an old Norwegian Fanuc manual, its G-code dialect used Q, F and L with G73 and G83, but no P. Do not see a point in quoting Norwegian only texts here. I did find this english page related to Fanuc, <URL: https://www.helmancnc.com/g83-peck-drilling-cycle-deep-hole-for-fanuc/ >: Z = Z-depth (feed to Z-depth starting from R plane) R = Position of the R plane Q = Depth of cut for each cutting feed (depth of each peck) F = Cutting feedrate K = Number of repeats (if required) In <URL: https://gcodetutor.com/fanuc-training-course/g73-g83-drilling-cycle.html > I find these: Z = Depth of hole I = Size of first cutting depth J = Amount of reduction of each depth of peck K = Minimum peck depth R = Retract value P = Dwell on last peck F = Feed rate Simliar in <URL: https://www.cnccookbook.com/g81-g73-g83-drill-peck-canned-cycle/ >: Z = Hole bottom R = Retract position in Z. Motions from initial Z to R are performed at rapids speeds. From R to hole bottom is done at feed speed. P = Dwell time at bottom of hole. Q = Depth to increase on each peck. F = Cutting feedrate L = Number of repeats Also found <URL: https://www.machinistguides.com/g83-code/ >: F = Feedrate G98 = Return to initial plane G99 = Return to R plane R = Position of the R plane (clearance level) X = Hole position in X-Axis Y = Hole position in Y-Axis Z = Position of the Z Axis at the bottom of hole Q = Depth to increase on each depth P = Dwell time at the bottom of the hole K or L = Number of cycle repetitions Is the peck clearence similar to R or K here, or is the P a new parameter? It seem to be in conflict with 'dwell time at the bottom' on some machines.

…

-- Vennlig hilsen Petter Reinholdtsen

[andypugh]

My understanding of these commits is that it makes the following statements in the docs a bit more explicit:
"Rapid up a bit." (G73)
"Rapid move back down to the current hole bottom, backed off a bit." (G83)
In that you can now decide how big "a bit" is.

In the Fanuc docs is says that this is a "machine parameter", and that is equivalent to what Chris' initial commit implemented.

[petterreinholdtsen]

[Andy Pugh]

My understanding of these commits is that it makes the following statements in the docs a bit more explicit: "Rapid up a bit." (G73) "Rapid move back down to the current hole bottom, backed off a bit." (G83) In that you can now decide how big "a bit" is.

Mine too. Note in the 1980 edition of the Fanuc doc I understand it to move completely out of the hole every time, so "a bit" is back to the position at the start of the drilling.

In the Fanuc docs is says that this is a "machine parameter", and that is equivalent to what Chris' initial commit implemented.

Yeah. The issue I wanted to raise is more if P is a good word for this parameter, as it seem to be used elsewhere with G83 to mean something different, not if it should be a machine parameter.

…

-- Happy hacking Petter Reinholdtsen

[petterreinholdtsen]

I suspect the "Rapid up .010 of an inch or 0.254 mm." part below should be modified too. The documented 0.1"/0.254mm do not seem to match the ini value default listed above.

[petterreinholdtsen]

I noticed in <URL: https://yewtu.be/watch?v=XRNnWAUoXrk > that FreeCAD have a 'Retract' length that can be set when specifying peck drilling. Is this the same as the R word in LinuxCNC? The comment in the video made me believe it was the length retracted per peck, which seem to be the same as the value discussed in this pull request. -- Happy hacking Petter Reinholdtsen

[andypugh]

I noticed in <URL: https://yewtu.be/watch?v=XRNnWAUoXrk > that FreeCAD have a 'Retract' length that can be set when specifying peck drilling. Is this the same as the R word in LinuxCNC?

Probably. I think the only way to be sure would be to change it and see how the generated G-code differs.
...
Amongst the ways to be sure include looking at the FreeCAD source code.

But I would expect that it is R

[andypugh]

Maybe it would be better to leave P available in case we want to add a pause at final depth.
However, there are not many letters available to use and inside the block structure only some letters are a suitable type.

double a_number;
double b_number;
double c_number;
double d_number_float;
int dollar_number;
double e_number;
double f_number;
int h_number;
double i_number;
double j_number;
double k_number;
int l_number;
int n_number;
double p_number;
double q_number;
double r_number;
double s_number;
int t_number;
double u_number;
double v_number;
double w_number;
double x_number;
double y_number;
double z_number;

abcuvwxyz are unavailable. As are F, S. N, T.
H, L, N, T are also the wrong data type.
R, L, Q are already in use.

which leaves D, E, I, J, K, P.

D might have been a better choice? (I have to take the blame here, as @rene-dev and I discussed this and it was I who decided that P was best)

[petterreinholdtsen]

I agree that it seem best to leave P unused to allow for a dwell/pause at the bottom of holes in the future. I came across <URL: https://www.haascnc.com/service/codes-settings.type=gcode.machine=mill.value=G73.html > and <URL: https://www.haascnc.com/service/codes-settings.type=gcode.machine=mill.value=G83.html > which describe the options used by Haas. G73: F - Feedrate * I - First peck depth * J - Amount to reduce pecking depth for pass * K - Minimum peck depth (The control calculates the number of pecks) * L - Number of loops (Number of holes to drill) if G91 (Incremental Mode) is used * P - Pause at the bottom of the hole (in seconds) * Q - Peck Depth (always incremental) * R - Position of the R plane (Distance above part surface) * X - X-Axis location of hole * Y - Y-Axis location of hole Z - Position of the Z-Axis at the bottom of hole G83: * E - Chip-clean RPM (Spindle reverses to remove chips after each cycle) F - Feedrate * I - Size of first peck depth * J - Amount to reduce peck depth each pass * K - Minimum depth of peck * L - Number of holes if G91 (Incremental Mode) is used, also G81 through G89. * P - Pause at end of last peck, in seconds (Dwell) * Q - Peck depth, always incremental * R - Position of the R plane (position above the part) * X - X-Axis location of hole * Y - Y-Axis location of hole Z - Position of the Z-Axis at the bottom of hole * indicates optional Could it be an idea to reuse Q instead of introducing a new parameter, in other words retract the peck depth (back to the earlier stop point) when pecking?

…

-- Happy hacking Petter Reinholdtsen

[petterreinholdtsen]

Via <URL: FreeCAD/FreeCAD#7185 > I discovered that FreeCAD calculate the default CHIPBREAKING_AMOUNT to Q * 0.05 if Q is set. Perhaps this is a better default for LinuxCNC too, instead of 0.05" / 1mm?

…

-- Happy hacking Petter Reinholdtsen

[andypugh]

instead of 0.05" / 1mm?

I think it is .01" or 0.254mm by default. 1mm seems too much for a default. I often peck with a Q of 1mm, in that case the system would spend equal time cutting air as cutting metal.

FSwizard suggests 0.05mm/tooth so my 1mm peck is only 10 turns, but that is a chip approx 50mm long.

[petterreinholdtsen]

[andypugh]

I think it is .01" or 0.254mm by default. 1mm seems too much for a default. I often peck with a Q of 1mm, in that case the system would spend equal time cutting air as cutting metal.

OK. I probably misunderstood the values of _setup.parameter_g73_peck_clearance and _setup.parameter_g83_peck_clearance of src/emc/rs274ngc/rs274ngc_pre.cc in the proposed patch, ie .050 for inches and 1 for the non-inches case.

…

-- Happy hacking Petter Reinholdtsen

[gmoccapy]

stuttgart meeting says we(andy) should change the letter.

[petterreinholdtsen]

[Norbert Schechner]

stuttgart meeting says we(andy) should change the letter.

Which letter should we change to?

…

-- Happy hacking Petter Reinholdtsen

[andypugh]

I think probably D. Unless anyone wants to propose another of the available and suitable pins:
D, E, I, J, K, P.

[petterreinholdtsen]

[Andy Pugh]

I think probably D. Unless anyone wants to propose another of the available and suitable pins: D, E, I, J, K, P.

Aha. As it look like a7909cb went into master using P for this, it is unclear how this will be done.

…

-- Happy hacking Petter Reinholdtsen

[andypugh]

Aha. As it look like a7909cb went into master using P for this

Well, that's confusing because I changed eveything to D and reworded the docs before pushing.