[Kiwi]

I would like to alter the tool approach to my part.

With the u..d.. set as;
RADID 100
Material Top 0
Cut Depth -5

The code produced;
G00 X0 Y0 Z100
G00 X40 Y50
G01 X40 Y50 Z-5 F50

As there is a distance of 105mm at F50 for the tool to travel this takes ages.
Can I get BCC to add a block 'G00 Z3' above the G01 block when generating the code and look like this.

G00 X0 Y0 Z100
G00 X40 Y50
G00 Z3
G01 X40 Y50 Z-5 F50

This would make life a little easier, thanks.

[tobyaxis]

I would like to alter the tool approach to my part.

With the u..d.. set as;
RADID 100
Material Top 0
Cut Depth -5

The code produced;
G00 X0 Y0 Z100
G00 X40 Y50
G01 X40 Y50 Z-5 F50

As there is a distance of 105mm at F50 for the tool to travel this takes ages.
Can I get BCC to add a block 'G00 Z3' above the G01 block when generating the code and look like this.

G00 X0 Y0 Z100
G00 X40 Y50
G00 Z3
G01 X40 Y50 Z-5 F50

This would make life a little easier, thanks.

You can use the Move to Point option in the CAM side. But first you have to create a point on the CAD side. This will help you to control the way BCC posts Start Positions.

[Kiwi]

Toby
Tried your suggestion as I understand it.
I created a point 3mm above my part and implemented 'Move to Point' but when I generate the code, as I have 100 in 'Rapid' the tool path moves up to this level and then down to Z-5 at the F50 feed rate.
I can insert the required block manually into the code but would prefer BCC to do this.
I think the Tool Depth Setting window should have provision to enter this figure.
Don't tell me Ver.2007 has this;-(

[tobyaxis]

Toby
Tried your suggestion as I understand it.
I created a point 3mm above my part and implemented 'Move to Point' but when I generate the code, as I have 100 in 'Rapid' the tool path moves up to this level and then down to Z-5 at the F50 feed rate.
I can insert the required block manually into the code but would prefer BCC to do this.
I think the Tool Depth Setting window should have provision to enter this figure.
Don't tell me Ver.2007 has this;-(

Yes, they both do. If you go into Setup (CAM Side) you can Create a Macro for your Start Position of a Tool. Mine looks like this because I wrote it out Manually and insert the XY Position.

I also included a Post Processor from BCC V2007. They did a very nice Job on these. Easy to Modify and Straight Forward.


Cheers Buddy!!!!!!

[Kiwi]

Toby
Made a Header macro but still unable to get exactly what I want.
My controller is a Fagor so not sure your Fanuc is of use.
My postprocessor (NC config) is a cfg format file. Do you know if this can be read as text file?

[tobyaxis]

Toby
Made a Header macro but still unable to get exactly what I want.
My controller is a Fagor so not sure your Fanuc is of use.
My postprocessor (NC config) is a cfg format file. Do you know if this can be read as text file?

Kiwi,

I'm not sure of the format in which BCC reads G-Code-to-Geometry. It might be NC or CNC.

Can you post a working G-Code File so we can look at it? Also there are Scripts that you can write to get what you want. I have seen your Script for the Ball Hitch 3D Spiral Interpolation. You shouldn't have too much trouble creating a script for your tool approach.

There is a Script Thread in CAD/CAM Trainer and the BCC Tech Support Forum

http://cadcamtrainer.com/forums/forumdisplay.php?f=79
http://216.117.147.20/bobcadsupport/...splay.php?f=12

Have you seen this Thread here in CNC Zone?
http://www.cnczone.com/forums/showthread.php?t=38996

[Kiwi]

Toby
I have a script which I use as a header which includes all the info I need up to the tool path.
BCC then generates the code less the G00 Z3 as shown in post #1
I also have a macro which I use to add the block G00 Z3. I need to go to the position in the code and run this macro.
I would rather do this than have to enter in X/Y coordinates.
I'm thinking I may not be able to make this process any simpler.

[tjones]

Have you tried running one script from another?

You can have the script sorta semi-automate the proccess.

[tobyaxis]

Have you tried running one script from another?

You can have the script sorta semi-automate the proccess.

Kiwi,

Try what Tjones said.

[Kiwi]

Thanks tjones and Toby for your help.
Not sure that is the answer as I need to enter the heading first.

N0000%NAME,MX
N0001 G51 E0.0001
N0002 S2000
N0003 M03 ;Spindle Clockwise
N0004 M08 ;Coolant ON
N0005 G00 Z100

Then BCC generates the code:

N0006 G00 X0. Y0.
N0007 G00 X72.658 Y-36.916
N0008 G01 X72.658 Y-36.916 Z0. F50
N0009 G41 G01 X79.503 Y-7.354 F800
N0010 G03 X73.658 Y0. I-5.845 J1.354

Now I manually delete Line N0006 and create a line space between N7 and N8
Run my macro which enters G00 Z3 in this line.

N0004 M08 ;Coolant ON
N0005 G00 Z100
N0007 G00 X72.658 Y-36.916
G00 Z3
N0008 G01 X72.658 Y-36.916 Z0. F50
N0009 G41 G01 X79.503 Y-7.354 F800

I believe I need to run the scripts separately as I need the BCC code after my heading and then do the Delete/Add to the BCC code.

Are you suggesting I should generate the code first then add my heading and do the adjustments?

[tobyaxis]

That is one way to do it Kiwi. What I prefer to do is call a personal heading

O0001
G0G17G40G49G80G90M5
G91G28Z0M9
G90
M1

N1(TOOL DESCRIPTION)
T1M6
G90G54G40G0X0Y0S2500M3
G43H1Z1.0
Z.1M8
>BCC GENERATED CODE FOR THIS TOOL IN LINES TO FOLLOW

G40G0Z.1M9
Z1.0M5
G91G28Z0
G49G90
M1

N2(NEXT TOOL SAME FORMAT AS ABOVE)

This makes programming a bit more uniform and easier to read. The above X0Y0 I usually change to the starting XY that BCC Generates. Yes it is a bit of work but wort it.

[tjones]

Use the script to change the lines.

Read the lines until the text = x0y0 then read that line and the next few lines into variables to replace with the needed output.

The script can be ran from the script that posts the code so you do not need to run it yourself.

I haven't done this in a while but there are several examples available.

If you need help figuring it out I could give it a try as I get time.

[Kiwi]

Toby: Thanks for your reply.
I don't see how your code speeds up the approach when the rapid level is set, say 100mm(4inches) above the part when the plunge feed is set at F50(F2).
My controller (Fagor) appears to use some different commands and find no spaces between commands hard to read. Age may have something to do with it too.
I guess it's what you get used to.

[Kiwi]

tjones: At my level of writing scripts, reading the code and modifing is a bit beyond me at present.
On reading the manual, I don't see a command to read the blocks.
A example script would be most helpful and appreciated.
Only when you have time as I'm in no hurry. Thanks for your offer.

[tjones]

I still do not know if this is the best thing for what you need. What I did was create my own start that generates this
G0Z0(home postion)
X0Y0(part home)
Z3.
then have Bobcad generate with rapid set in up down to .1 above the part

anyhow here is a script you could use to find and change
change the X??? to what is in the program
and the output to what you want it changed to

You can also change the output text to a variable for operator input if you like as well or read from numbers in other lines that can be stored in variables.

'FIND ??? AND REPLACE SCRIPT BY TIM JONES'


NCEdit Line = 1
NCEdit Output,Line = i

NCEdit Output, NumLines = nl

NUMLINES = nl - i

For Index = 1 To (NUMLINES + 1)
	NCEdit Line = i + (Index - 1), Output, Text = txt
	If InStr(txt,"X???") Then 
		txt = "X1."
		NCEdit Line = i + (Index - 1), Text = txt
		Index=NUMLINES+1
	end if
Next Index

[Kiwi]

tjones
Thanks for the sample script. I'll work on it tonight and see if I can get it to work.

[Kiwi]

tjones
Worked on the script and got it to do what I require.
Not sure this is good script writing practice but it works.
====================================
NCEdit Line = 1
NCEdit Output,Line = i

NCEdit Output, NumLines = nl

NUMLINES = nl - i

For Index = 1 To (NUMLINES + 1)
NCEdit Line = i + (Index - 1), Output, Text = txt

Mystr = Left(txt,5)

If Instr(Mystr,"N0007") Then
txt1 = txt
txt2 = "N0007 G00 Z3"

NCEdit Line = i + (Index - 2), Output, Text = txt
NCEdit Line = i + (Index - 2), Text = txt1

NCEdit Line = i + (Index - 1), Output, Text = txt
NCEdit Line = i + (Index - 1), Text = txt2

Index=NUMLINES+1
end if

Next Index
========================================
This is after runing the macro:

N0005 G00 Z100
N0007 G00 X3. Y0.
N0007 G00 Z3
N0008 G01 X3. Y0. Z0. F50

Thanks for your help.

[tjones]

Actually it looks pretty good. Obviously you know your way around some programming to have done this. Most people would have asked for more help until I completed the script from start to end.

Do you like the way it starts from the top of the program instead of where the cursor is located? This way it can be ran from another script. So what you can do is make a script to place in your macro menu.

Call it 'Run and Replace' if you like. But in it have the 'run all' maco run and then run the 'replace' script you now have. This makes the scripting very automated in that it will combine the sepperate steps into the one selection.

BTW: The 'If Instr' search it uses can find any text within the entire line. So you do not need to be set to the line number to have it work correctly. If you knew which line number you could have set the cursor position to that number instead of searching the lines. (The top line in the script sets the line where the cursor is located.)

[tjones]

Here is a way if you know what line numbers to read and write to instead of searching.

NCEdit Line = 6, Output, Text = txt
txt1 = txt
txt2 = "N0007 G00 Z3"

NCEdit Line = 5, Output, Text = txt
NCEdit Line = 5, Text = txt1

NCEdit Line = 6, Output, Text = txt
NCEdit Line = 6, Text = txt2

[Kiwi]

tjones

I do a bit of programing with VB6 so this is not entirely new to me.

I'm quite happy to run as a standalone macro. There maybe times when I don't want this setup. As this correction is within the first 10 lines I will modify the loop.
I'm not completely happy with the search for a line number when the data I'm looking for is the X0 Y0.
I couldn't see a simple solution because the script would find the X0 Y0 but I also needed the info in the next line. I'll look to improve it.
I was being distracted while doing this as I was watching the America's Cup Yacht racing live at 1am -3am local time.
Thanks again for your help, It's nice to have somebody arround that know a little bit more.