Rapid Speed in Sheetcam Job Report

[Reb0rn]

When i make a job report on Sheetcam, i see the total run time, but it is way off(on a certain job the actual time was 1.5x calculated). I checked the cutting speed, and that is 100% on spot. So next step i checked if Sheetcam calculated each pierce, and yes it does. Next i was wondering what my rapid speed was, but i cant seem to find it in Sheetcam or in my Mach3 controller.

In Sheetcam job report i said 2000 mm/sec, wich is not really fast, so i actually doubt that the rapid speed is actually slower than 2000... But still i want to check this.

I want the time to be accurate, so i can pre-calculate the price of the job.

Any suggestions?

[acourtjester]

In Mach you can change the rapid speed by adjusting the Velocity and Acceleration, you want this to be fast as it can but without motor stalling.

[Reb0rn]

So it is a calculation of 2 numbers?

I guess i should place 2 objects 1m apart of each other, and than use a stopwatch and calculate it.

But i believe it isn't slower than 2000 mm/min, so there must be another problem with it.

[adbuch]

In Mach you can change the rapid speed by adjusting the Velocity and Acceleration, you want this to be fast as it can but without motor stalling.

Tom - would his rapid speed show up in the G-code as G0 x.xxx? Or is overridden by the controller?
David

[acourtjester]

Reb0rn to test the speed of an axis you can assign a distance with g-code line of code, like 30 inches. I think the g-code would be G1 X30 F100 to travel 30 inches in 1 minute time. In Mach if you do not give a F value it will travel at the last F commands speed only with a G1 command.

David The max speed established in the calibration will be the G0 speed, G1 is controlled by the F value assigned in the G-code. Or if a command line written in the MDI location used for single actions entered as a move to a location for testing or repositioning to another coordination.

[adbuch]

Reb0rn to test the speed of an axis you can assign a distance with g-code line of code, like 30 inches. I think the g-code would be G1 X30 F100 to travel 30 inches in 1 minute time. In Mach if you do not give a F value it will travel at the last F commands speed only with a G1 command.

David The max speed established in the calibration will be the G0 speed, G1 is controlled by the F value assigned in the G-code. Or if a command line written in the MDI location used for single actions entered as a move to a location for testing or repositioning to another coordination.

Tom - yes I understand G0 = rapid and G1 = feed. Assuming his g-code matches the piece he is cutting, then unless there is some override from the controller the g-code will tell these speeds (assuming his system is calibrated with proper turns ratios settings for his physical hardware).

My question was - does his system have this override capability (or not). With my cnc machining centers I can manually override the feed rate and rapid speed with knobs on the control panel. These typically range from 0% override 10% increments up to 200%. I believe I can accomplish similar with my Mach3 control for my cnc router and Centroid Acron CNC12 that runs my other cnc router.

So if he has this capability with his system, then he would need to make sure overrides are set to 100% for rapids and feeds.

David

[Reb0rn]

Well for me its not a problem if the rapid speed is not at its maximum. Its the thing that i want an accurate job report in sheetcam, and for that i wanted to know if i could see somewhere the rapid speed.

I will do a test for that.

If anyone has other idea for job time (without real cutting), let me know.


a small extra question:
im looking into mach3 CV control. it has the following:

plasma mode OFF
CV Dist Tolerance 25
G100 addaptive nurbsCV ON
Stop CV on angles OFF

are these correct settings?

[acourtjester]

First off I made a mistake in the single line G-code above to check the speed the value for F in either inches or MM per time. That is to check it use a distance that equals the speed and check if it moves that distance in that time. Meaning you say X40 F40 it should move the 40 in one minute.
I have not seen a percent increase for speed/feeds in Mach, I have seen it in Lightburn for both speed and power. I am not an expert and only go by my experiences. I did look in sheetCam for a rapid speed setting and did not see one, does not mean there is not one there. My memory does tell me I have seen one somewhere, but cannot say where, it seems there should be one. In LinuxCNC there is one you can manually change in the INI file.
looking now this is what I found.
https://www.plasmaspider.com/viewtopic.php?t=7180
and

[adbuch]

I have not seen a percent increase for speed/feeds in Mach .......

Tom- I have Mach3 on one of my Avid tables and it works as shown below for manual feedrate override. It affects both rapids and feeds.
David

https://allcnc4you.wordpress.com/2013/1 ... e-in-mach/

mach feedrate override 2.jpg (41.43 KiB) Viewed 4844 times

mach feedrate override 2.jpg (41.43 KiB) Viewed 4844 times

[Larry83301]

You could try here - - -

Motor tunning Mach3.JPG (66.97 KiB) Viewed 4842 times

Motor tunning Mach3.JPG (66.97 KiB) Viewed 4842 times

[acourtjester]

Good find thanks David

[adbuch]

Good find thanks David

Tom,
I often kick the feedrate down when doing trial test runs before cutting. Makes it easier to pause if I've mis-programmed and heading for one of my work holddowns. Same with my cnc turning center (lathe) and cnc machining center (mill). Better safe than sorry.
David

[cutnweld]

In sheetcam when you make your job report you can tell it your table speed. It will not change how fast your table moves but will help the estimating be more accurate. Your rapid commands are by default a G00xxx etc and will move whatever maximum velocity you have set in Mach3 under the motor tuning tab.

[TJS]

Doesn't acceleration settings come into play in order to get to the desired speed. I know in command CNC there are setting for this in the configurator. I would think this would affect the time as well to go from point A to B. How does sheetcam know what the acceleration settings are in Command CNC. I don't think it does. Not sure about Mach.

[TJS]

delete

[TJS]

delete

[34by151]

I dont have any machines running Mach3 anymore but I do have customers using it.
To get around the issue I do a few things in Mach and some in the post processor

In Mach mac sure the motor tuning is done so you can access your best feed rate

In the Post Processor add an "F" command on the line line before the the G00
Make sure all the rest of the moves in the Post processor have the F command included

N2700 F8000
N2710 G00 X1702.2711 Y697.9778

I also use the Post processor to calculate the Time and Length of the moves and pierce.
I Include the totals at the end of the gcode as well as in a separate file (with the tap file)
This time and distances are accurate to a few seconds to the machine run times and can be used for billing

N59420 (*********************************************)
N59430 (Material Size)
N59440 (Length = 2125.32 mm)
N59450 (Width = 1160.01 mm)
N59460 (Area = 2465380 mm2)
N59470 (Area = 2.4 m2)
N59480 (*********************************************)
N59490 (Machine Travel Length)
N59500 (Line Cutting = 49064 mm)
N59510 (ARC Cutting = 17596 mm)
N59520 (RAPID Moves = 67677 mm)
N59530 (CUTTING Length (Total) = 66660 mm)
N59540 (TOTAL Length = 134337.25 mm)
N59550 (*********************************************)
N59560 (Machine Time)
N59570 (Line Cutting = 41.9 Minutes)
N59580 (ARC Cutting = 26.15 Minutes)
N59590 (RAPID Moves = 8.46 Minutes)
N59600 (PIERCE time = 14.25 Minutes)
N59610 (Cutting Time = 68.05 Minutes)
N59620 (Total Time = 90.76 Minutes)
N59630 (*********************************************)
N59640 (Torch)
N59650 (PIERCES = 171)
N59660 (RAPID Speed = 8000 mm/Min)
N59670 (*********************************************)

[adbuch]

I dont have any machines running Mach3 anymore but I do have customers using it.
To get around the issue I do a few things in Mach and some in the post processor

In Mach mac sure the motor tuning is done so you can access your best feed rate

In the Post Processor add an "F" command on the line line before the the G00
Make sure all the rest of the moves in the Post processor have the F command included

N2700 F8000
N2710 G00 X1702.2711 Y697.9778

I also use the Post processor to calculate the Time and Length of the moves and pierce.
I Include the totals at the end of the gcode as well as in a separate file (with the tap file)
This time and distances are accurate to a few seconds to the machine run times and can be used for billing

N59420 (*********************************************)
N59430 (Material Size)
N59440 (Length = 2125.32 mm)
N59450 (Width = 1160.01 mm)
N59460 (Area = 2465380 mm2)
N59470 (Area = 2.4 m2)
N59480 (*********************************************)
N59490 (Machine Travel Length)
N59500 (Line Cutting = 49064 mm)
N59510 (ARC Cutting = 17596 mm)
N59520 (RAPID Moves = 67677 mm)
N59530 (CUTTING Length (Total) = 66660 mm)
N59540 (TOTAL Length = 134337.25 mm)
N59550 (*********************************************)
N59560 (Machine Time)
N59570 (Line Cutting = 41.9 Minutes)
N59580 (ARC Cutting = 26.15 Minutes)
N59590 (RAPID Moves = 8.46 Minutes)
N59600 (PIERCE time = 14.25 Minutes)
N59610 (Cutting Time = 68.05 Minutes)
N59620 (Total Time = 90.76 Minutes)
N59630 (*********************************************)
N59640 (Torch)
N59650 (PIERCES = 171)
N59660 (RAPID Speed = 8000 mm/Min)
N59670 (*********************************************)

Thanks for sharing that! Very good information to know. I still run Mach3 on one of my tables.
David

[34by151]

The Key with Sheetcam and time estimates are the THC Probe Time and the Rapid Times
Calculating the actual Move,Rapid and pierce distances are done in the sheetcam post processor

In each function (OnRapid,OnMove,OnArc and OnPenDown)
I calculate the length in a local variable
I then add this length to a total length and the length * feed to a total time

This gives an accurate time and distance
I keep the totals for Rapid, Arc and Line moves in separate totals till the end
I can then tally the totals for each and add then up for the total machine time and distance

I also account for the extra time taken when slowing down in the corners.
As each line of gcode is generated we add to the tally.
So as the line has a slower feed rate it adds more time

The above Postprocessor uses an external standalone THC
Mach3 is just doing the XY all the Z is done with the THC

Mach3 has some extra Mcodes added

One is used to enable the THC auto signal
Its just used at the start of the Gcode to make sure the THC button is enabled
This saves on an operator mistake
THC needs to be on to make Mach3 M03 code to wait for the ARC OK from the THC
THC does the Ohmic probe and pierce before sending the ARC OK

Corner slowdown is done in Sheetcam rules
The slowdown rules have begin and end code snippets
The snippets turn on and off and output
This is wired to the THC corner signal.
This stops the THC moving the Z and diving with the slowdown

I account pierce times by using the pierce time from sheetcam and adding extra time for the IHS probe and torch retract.
This is timed and added to a variable in the Post processor
Pierce time is in the tool setting of sheetcam

I also calculate the job boundaries at the start of the post processor
I use this to enable the Laser Pointer and run the pointer around the job
This is done at the start of the job to make sure the job will fit on the sheet

The sequence is
Start Job (pendant start button)
IHS probe and set 0,0
Wait for keypress (pendant button)
Run Laser pointer around Job
Wait for keypress (pendant button) or Cancel Job
Start Cutting

Happy to send a copy of the Post processor if anyone wants a copy

[Thielmetalfab]

Would love to setup code in sheet cam to to do a test with laser pointer on sheet before actually cutting.
Using mach 4 though .
Would your code for post processor work in mach4

[34by151]

It should work in Mach4 but may need some changes for your setup however you can use the code to get a proper estimate

i also have a "border trace" generated in Sheetcam

This calculates the X and Y edges, turns on the laser pointer and moves around the border
Once this is done it pauses till a "confirm" button is pressed

I dont use this much as I also put code in Mach to do the same

Send me a PM and i will send you a copy

[Thielmetalfab]

Would like to do the code in mach4 as well.
But know mach4 uses lua . So thats prolly quite different?

[34by151]

You could modify the Mach3 code for MAch4 easily as its not that complex

I also do it directly in the sheetcam post processor, that will work with any control system as it just generating G00 movements


Add this to the OnInit() function in your sheetcam post

jobMin = sc.Coord2D(1e17,1e17)
jobMax = sc.Coord2D(-1e17,-1e17)
sc.Parts:Get():GetExtents(jobMin, jobMax)
MatSizeL = string.format("%.2f",((jobMax.x - jobMin.x) *scale))
MatSizeW = string.format("%.2f",((jobMax.y - jobMin.y)*scale) )
post.Text ("M821 (Turn on Laser Pointer)\n")
post.Text ("G0 X",MatSizeL," Y0.0 (Trace First Side)\n")
post.Text ("G0 X",MatSizeL," Y",MatSizeW," (Trace Second Side)\n")
post.Text ("G0 X0.0"," Y",MatSizeW," (Trace Third Side)\n")
post.Text ("G0 X0.0 Y0.0 (Trace Forth Side)\n")
post.Text ("M831 (Await Pendant Key)\n")
post.Text ("M822 (Turn off Laser Pointer)\n")


Change the M821/M822 to the M codes to turn on/off your laser pointer
Also the M832 is optional. its an M code that just waits for an input to go active
This causes the the job to wait till the key is pressed or you stop the g-code

If you cant do a keypress change the line to a G04 Pxxxx pause with enoughh time for you to abort if needed