PDA

View Full Version : Edge finding. Center.



tantemay
12-13-2018, 05:11 AM
Is it possible to measure the center with a manual / mechanical edge finder? Like Estlcam?

awerby
12-13-2018, 03:08 PM
The center of what - a hole? You can do that if your edge finder has a pointy end that fits it.

tantemay
12-13-2018, 05:04 PM
A circle, a rectangle or whatever.
For me it's about whether you can drive the axes manually, and then confirm the position. As is possible with Estlcam.

PlanetCNC
12-18-2018, 08:35 AM
Sure, you can use PlanetCNC TNG and probe for your measurement application.

TNG by default already offers few measurement procedures such as, measuring of hole center, work offset -> corner/edge of workpiece etc...

You can can create your own measuring procedure by writing your own measurement g-code program that would perfectly suit your needs.

Of course you can also move your machine manually and using probe. When probe trips you can either set new work position, save coordinate positions etc...

tantemay
12-22-2018, 06:57 AM
Thanks for the many answers.
I think I was not understood correctly.
I would like to manually touch the edges of the workpiece, for example, a cylinder. And the CNCUSB TNG software then calculates the center of the cylinder based on 3 points.
The same with four points at a rectangle / square

The measuring points are entered manually each time.
That means you drive the machine with the jogpad or the handwheel to a position and save this point, the same then with the other measuring points.

I would like to touch the positions without an electronic probe. So with a manual

In short, I would like to touch the points A, B and C manually with a manual probe. And the control software then calculates midpoint (M)

tantemay
12-23-2018, 05:25 AM
I also miss the functions for measuring the midpoint using the outer circle.

Or I'm just too blind to find that.

tantemay
12-25-2018, 06:40 AM
Sure, you can use PlanetCNC TNG and probe for your measurement application.

TNG by default already offers few measurement procedures such as, measuring of hole center, work offset -> corner/edge of workpiece etc...

You can can create your own measuring procedure by writing your own measurement g-code program that would perfectly suit your needs.

Of course you can also move your machine manually and using probe. When probe trips you can either set new work position, save coordinate positions etc...
I paid money for the hardware and software. I think my paid money works.
Now I was told to write scripts / programs to work like my old free software, which can do it with a $ 10 hardware?

Is that the answer from Planet CNC Support?

PlanetCNC
12-26-2018, 04:32 PM
Script for 4 point circle center measuring with probe is included with TNG.

In more than 10 years we never got request for 3 point manual circle center.

Because it is possible to use scripts this can be implemented and you are not limited. But if you have satisfactory solution for 10$ then go with it. It is certainly easier than programming scripts in g-code.

tantemay
12-26-2018, 05:52 PM
I think you do not understand it.
I want to get the midpoint from the outside of a body. Not from the inside of a hole.
That was possible with the old controller software. With the TNG, this is only possible with a hole.
I do not care if this is done with 4 or 3 measuring points.

tantemay
01-01-2019, 01:11 PM
Hello.

I have now clicked the script myself. Someone who, like the developer of the software, knows what the GCode does mean, that would have been very easy. Anyway, I think he just did not understand what I wanted.

When you start the script it asks for the diameter of the workpice in the X and Y axis

Before you start it, the probe must be approximately centered on the left side of the workpiece. (On the picture you can see which position is meant.)


The sensor starts from current Z position to + X. As soon as he has a measuring point, he drives back 10mm in the direction of -X. Then Z is raised by 20mm.
Then the probe is moved in the + X direction by the entered value diameter X + 20mm
The probe is lowered to the initial Z position.
From there it is moved in -x direction until a measuring point is reached. Now it will be moved 10mm back towards + X, and 20mm + Z direction.
The script now calculates the midpoint between the 1st and 2nd measurement points and moves the sensor to this position.
The script continues with the Y axisand so on. ...

The workpiece size is limited to 200 mm in the script.
If you enter a larger value, automatically 200mm is assumed. There is no error message.
In line 2 and 3 you can adjust the maximum.

The script must be in / Applications / Planet-CNC / Profiles / Default / Scripts
be placed.
The name must be "UD followed by a number".
So, for example UD6.gcode

In the first line you can change the 0 to a 1. Then the script is not started immediately, but only loaded. It must then be started with the play button.

The script is loaded in the TNG software via the menu / Machine / User Defind.






(name,Center Outside, 0)
(dlg,Diameter X, 2, 30, 0.1, 200)
(dlg,Diameter Y, 2, 30, 0.1, 200)

O<PlanetCNC> if[[#<_sensor1_pin> GT 0] OR [#<_sensor2_pin> GT 0]]
M70 (store state)
G90 (absolute mode)
G94 (units per minute mode)
F#<_speed_probe> (probe speed)
#<DiamX> = [[#<_Center_Outside-Diameter_X>] +20]
#<DiamY> = [[#<_Center_Outside-Diameter_Y>] +20]
#<RadiusY> = [[#<_Center_Outside-Diameter_Y>] /2+10]

;store start position
#<startx> = #<_x>
#<starty> = #<_y>
#<startz> = #<_z>

;probe in X+ direction
G38.2 X+10000
#<px1> = #<_probe_work_x>
G91 (incremental mode)
G00 x-10
G00 Z+20
G90 (absolute mode)

;go to 2. position
G91 (incremental mode)
G00 X#<DiamX>
G90 (absolute mode)
G00 Z#<startz>

;probe in X- direction
G38.2 X-10000
#<px2> = #<_probe_work_x>
G91 (incremental mode)
G00 X+10
G00 Z+20
G90 (absolute mode)

;calculate X center
#<cx> = [[#<px1> + #<px2>] / 2]
;go to center
G00 X#<cx>

;go to 3. position
G91 (incremental mode)
G00 Y#<RadiusY>
G90 (absolute mode)
G00 Z#<startz>


;probe in Y- direction
G38.2 Y-10000
#<py1> = #<_probe_work_y>
G91 (incremental mode)
G00 Y+10
G00 Z+20
G90 (absolute mode)

;go to 4. position
G91 (incremental mode)
G00 Y-#<DiamY>
G90 (absolute mode)
G00 Z#<startz>

;probe in Y+ direction
G38.2 Y+10000
#<py2> = #<_probe_work_y>
G91 (incremental mode)
G00 Y-10
G00 Z+20
G90 (absolute mode)

;calculate Y center
#<cy> = [[#<py1> + #<py2>] / 2]
;go to center
G00 Y#<cy>

;set work position xy to Zero
G92 X0 Y0


F#<_speed_feed> (feed speed)
M70 (restore state)
O<PlanetCNC> else
(msgdlg,Sensor is not configured)
O<PlanetCNC> endif

Eatonbrayer
01-02-2019, 02:35 AM
This touches an inadequacy that I have. I cannot currently fully understand scripting.
Where would a "mature student" begin to find a suitable learning resource please?
Even if someone would be kind enough to do a line by line work through, as "Tantemay" has helpfully touched upon here, it would be a very useful start for me and I would imagine others.

tantemay
01-02-2019, 06:29 AM
The scripting language is O Codes (http://linuxcnc.org/docs/html/gcode/o-code.html) (yes, like in LinuxCNC) and G-code, as far as I understand it.
One may correct me that is not true.
I can not say if it's actually the same syntax.
It would be very nice if the developer would say something "concrete".

I would like to explain the script line by line.
The difficult or tedious would be only to translate it from German to English.
But I have to say I learned that only through trial and error.
Last time I programmed something in Basic / Pascal 30 years ago.

Eatonbrayer
01-02-2019, 08:17 AM
Yes I have enquired to PlanetCNC support but the answer was very grey. It is as if they wanted to keep it to themselves. Thank you for the link.