Tool Radius Compensation Program

Submit any comments, issues or requests relating to the use of VR Milling Version 5 and 2

Moderators: Martin, Steve, Mr Magoo

Post Reply
SANJAY SURI
Posts: 3
Joined: Thu 08 May , 2014 15:13 pm
Hardware/Software: Novamil plus VR Milling 5
Novaturn VR Turning 5
Router 2600 Pro (4 axis)
QuickCAM2D Design
QuickTurn2D Design
QuickCam Pro
Quick Cam4D

Tool Radius Compensation Program

Post by SANJAY SURI » Wed 04 Jun , 2014 10:16 am

Hi,

I have written the simple program below to show our students how to use the G41/G40 for tool radius compensation:

[BILLET X80 Y80 Z10 (tool diameter 6.35mm radius 3.175)
(Required compensated toopath A-D: A=X23.175/Y23.175; B=X56.825/Y23.175;)
(C=X56.825/Y56.825; D=X23.175/Y23.175)
N010 S2000 M03 T01
N020 G00 X20 Y10 Z10 (CHANGING Y HERE MAKES X VAL BELOW CHANGE)
N030 G41 X23.175 Y20 Z1 (ONLY WORKS WHEN COMPENSATED X VAL INSERTED)
N040 G01 Z-1F40
N050 X60 (COMPENSATED CORRECTLY)
N060 Y60 (COMPENSATED CORRECTLY)
N070 X20 (COMPENSATED CORRECTLY)
N080 Y23.175 (ONLY WORKS WHEN COMPENSATED Y VAL INSERTED)
N090 G40 X0 Y0 Z10
N100 M05

Can you please check if this is how you would structure such a program to cut a pocket 40mm x 20mm using tool radius compensation?

I cannot get my head around the following:

-Why does changing the value of Y in line N020 change the value of X in line N030?
-Why is the value of X in line N030 not compensated for automatically - I have to put in the
compensated value myself?
-Why is the value of Y in line N080 not compensated for automatically - I have to put in the
compensated value (23.175) myself?

If possible I would be grateful if someone could look at this today as I would like to cover this topic with my class this evening.

Cheers

Sanjay

User avatar
Steve
CNC Guru
CNC Guru
Posts: 1432
Joined: Tue 21 Feb , 2006 16:15 pm
Location: Denford UK

Re: Tool Radius Compensation Program

Post by Steve » Wed 04 Jun , 2014 12:49 pm

What version of software are you using? There have been changes in VR Milling 5 to resolve some issues. Versions before 5.48 need the update.

The current version is available to download.

http://website.denford.ltd.uk/index.php ... -downloads.

SANJAY SURI
Posts: 3
Joined: Thu 08 May , 2014 15:13 pm
Hardware/Software: Novamil plus VR Milling 5
Novaturn VR Turning 5
Router 2600 Pro (4 axis)
QuickCAM2D Design
QuickTurn2D Design
QuickCam Pro
Quick Cam4D

Re: Tool Radius Compensation Program

Post by SANJAY SURI » Thu 12 Jun , 2014 15:59 pm

Hi,

I am using version 5.54 which I believe is the latest version so please have a look at my program again and advise.

Also something else cropped up in my lesson yesterday which I would appreciate your help with:

I wrote a simple program to engrave the letter 'A' onto my billet using a 2mm slot drill. I then wanted to go over the cut with an end mill (tool 3) and finally a bull nose cutter (tool 2). I would like to know if there is a way to run the same program with the 3 different tools with the same speen and feed rate without having to repeat all the coordinates 3 times i.e. some kind of canned cycle/ subroutine - there must be a way!

Here is my code:

Billet X60 Y80 Z10
Start of main program - cut with slot drill)
N010 G90 T01
N020 G00 X0 Y0 Z1.0
N030 M03 S2500
N040 X10 Y20 Z1
N050 G01 Z-1 F254.00
N060 X30 Y70
N070 X40 Y45
N080 X20
N090 X40
N100 X50 Y20
N110 G00 Z10
N120 G28 X0 Y0 Z0
N130 M01
(end of main program)
N140 M06 T03 (start of 2nd cut with end mill - repeated coordinated, speeds, feeds)
N150 G00 X0 Y0 Z1.0
N160 M03 S2500
N170 X10 Y20 Z1
N180 G01 Z0 F254.00
N190 X30 Y70
N200 X40 Y45
N210 X20
N220 X40
N230 X50 Y20
N240 G00 Z10
N250 G28 X0 Y0 Z0
N260 M01 end of 2nd cut)
N270 M06 T02 (start of 3rd cut with bull nose - repeated coordinates, speeds feeds)
N280 G00 X0 Y0 Z1.0
N290 M03 S2500
N300 X10 Y20 Z-0.5
N310 G01 Z0 F254.00
N320 X30 Y70
N330 X40 Y45
N340 X20
N350 X40
N360 X50 Y20
N370 G00 Z10
N380 G28 X0 Y0 Z0
N390 M01 (end of 3rd cut)
N400 M05
N410 M30

User avatar
Steve
CNC Guru
CNC Guru
Posts: 1432
Joined: Tue 21 Feb , 2006 16:15 pm
Location: Denford UK

Re: Tool Radius Compensation Program

Post by Steve » Thu 12 Jun , 2014 16:37 pm

If you set the file sourse to full editor from the file menu then you can copy a block of lines and paste the them in the editor.

Then all you have to do is edit the toolchange lines

User avatar
Steve
CNC Guru
CNC Guru
Posts: 1432
Joined: Tue 21 Feb , 2006 16:15 pm
Location: Denford UK

Re: Tool Radius Compensation Program

Post by Steve » Thu 12 Jun , 2014 16:52 pm

Here are the notes in relation to the use of cutter compensation from the help file.

Can you ensure the requirements are met?
Can you produce a drawing of the shape required and also ensure the previous G01 move is greater than the cutter radius. In the sample the move seems to be the same as the radius.



Cutter Compensation Start-up (G41-42).
The operation instructing a machine to switch to cutter compensation mode is called the start-up block, or ramping on block. The start-up block is used to allow the tool time to change from moving along the programmed path line to following either side of the programmed path line.

The start-up block should satisfy the following points:

1) A G41 or G42 code must contained in the block, or specified in the previous block.

2) A GØ1 X, Y, or X and Y move is specified in the block and the distance of the linear move must be greater than the tool radius.

3) The tool radius value, "R", entered into the tool offsets table must not be ØØ.

Note 1.

A GØ2 or GØ3 circular interpolation command cannot be specified in the start-up block.

Note 2.

In cutter compensation start-up, two blocks are read into the machine controller. The first block is performed and the second block is entered and held in memory.

In subsequent compensation moves, two blocks are read in advance, so the machine controller has the block currently being performed and the next two blocks in memory.

This is because cutter compensation always needs to know what happens in the move following the one being currently performed. The machine controller can plan ahead to calculate the correct end position for the current move, that will also be the correct start position allowing for cutter compensation, for the next move.

Note 3.

The codes G4Ø, G41 and G42 are modal, belonging to the same modal family. They are incompatible with each other on the same block.

Post Reply