[skipper]

Hi Guys,

I am using Mach3 as my Rockcliff Router control software. When I am setting up my CAM part, FANUC is I believe the defaut controller listed in SolidCAM. Is this what I should be using for Mach3?

thanks,
skipper

[dhenry]

I created my oun mach 3 processor to suit my needs. I copied the fanuc and the edited until I was happy.

Doug Henry

[Adam Hubert]

As Doug mentioned modifying posts in SolidCAM is not really all that difficult. Perhaps not possible for a beginning CNC machinist but an experienced user of non-conversational G-Code style CNC should be able to do it. Keep it simple getting started. The logic in these files related to multi-axis indexial, 4/5 simultaneous, Mill-Turn, and so on can at times get incredibly complex.

In your GPPTool directory you have a bunch of files that end in either *.mac or *.gpp. For example Fadal6030.mac and Fadal6030.gpp, fanuc.mac and fanuc.gpp, Haas_3d.mac, Haas_3d.gpp, etc. These *.mac files are man readable ascii text files that can be called up in any text editor. The mac, aka as machine file, aka as pre-processor is what you choose at the very beginning after File New Milling, File File New Turn, and so on. In the dialog box at the top left it's called CNC-Controller.

The mac file tells or flavors the internal guts of SolidCAM general information about your machine, how many axes it has, do or don't you want to use sub-programs, do or don't you use cutter compensation, spindle speed maximum values, feed rate maximum values, and much more. General information about your machine and what general programming techniques you use.

You then in the processing, aka tool path creation, aka operation creation stage create all of your coordinate systems, stock model, target model, tools, tool paths, and so on. Internally SolidCAM keeps track of all that you tell it in in a file that SolidCAM calls a PJ file. Many systems years ago used to call this a CL file.

When done with all of the above, simulation looks good, and you click on generate G-code SolidCAM presents the instructions and associated values from the dialog boxes from the PJ file to the *.gpp file that has the calls and the logic to create the G-Code. You will see that the *.gpp file is also an ascii readable text file.

One this is all understood then you can begin to think about editing, tweaking, to to get output the way you like it for your machine. Most important is to understand where all the G-code comes from. Or said another way what area in the gpp creates or contains the logic that is driving the output of the code of concern (perhaps an area you need to change). Very useful to sort this out is a command called trace in the gpp file. Essentially you enter into the gpp file a command that kicks it into a diagnostic mode that outputs some extra information in your G-Code that tells you where the G-code output is coming from. Now you know where to go in the gpp file to make changes.

It will look something like the following

; GPPL variables
pre_processor = 'FANUC'
numeric_def_f = '5.3'
integer_def_f = '5.0(p)'
gcode_f = '2.0(p)'
mcode_f = '2.0(p)'
xpos_f = '5.3'
ypos_f = '5.3'
zpos_f = '5.3'
feed_f = '4.3(p)'
tool_diameter_f = '5.3/1'
blknum_f = '5.0(p)'
blknum_gen = false
blknum_exist = true
blknum = 1
blknum_delta = 1
blknum_max = 32000
trace 'all':1

trace 'all':0 will output normal G-code without any diagnostics. Replace the 0 with either 1, 2, 3, 4, or 5 for differing levels of diagnostic information.

This is all documented in the GPPTool help file but sometimes it's confusing and helps to have a bit of guidance to get started.

I created my oun mach 3 processor to suit my needs. I copied the fanuc and the edited until I was happy.

Doug Henry

[dhenry]

The mach web site says use the fanuc processor as their is no post processor for solidcam.

I did as follows:
1. Copied the two fanuc files and renamed them as mach3.
2. I then loaded them as my default processor.
3. Checked they worked.
4. Examined the G Code produced on a simple shape.
5. Loaded it into mach3 and viewed the tool path.
6. If it is full of looping circle change the general property in Mach3 to W mode to incremental.
7. Delete part of the post processor you think you do not need or change a setting. Be carful to keep several backups so you can roll back if necessary.
8. Then go back to step 4 and test.

Make small changes so you post processor evolves. That fact you do not know what the effect of your change does not matter, for if you make small changes and check you can undo them.

Doug Henry

[aquatix]

Can the default Fanuc use 4 axis simulatneously with some modification?
I use the Facuc with Mach 3 and no problem . but I cannot make it work with the 4 axis

[aquatix]

is there a post processor for Solidcam 4 axis ?