Tool approach Tool Path

[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]

Originally Posted by 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.

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]

Originally Posted by 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;-(

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]

Originally Posted by 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?

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]

Originally Posted by tjones 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.