Part 18

The programs

Roughing, finishing and chamfering are typical machining operations. In reality, it is not only the periphery and the edges of any profiles and pockets which are first roughed out then finished, but any subsequent chamfers which are also roughed then finished. The chamfering operation may produce a fairly large chamfer but can also be used to just kiss the edges, effectively doing much of the deburring that otherwise might have to be done by hand once the machined workpiece has been removed from the mill.

The programs for MACH3 can be downloaded from the list below.

There are several programs here, and notes on each.

Be aware that the average length of each program is a little over 5000 lines.

Be aware, too, that licences for MACH3 will not be available for much longer, and if you have been reading the Newsletter, you will know that MACH4 is a different animal, so my advice, if you are running the demo version of MACH3 on XP is to buy a licence now. I do not get commission, and have no connection with the company marketing MACH3, so this is simply my intended-to-be-helpful advice.

Profile

    Roughing with 6mm end mill

    Finishing with 6mm end mill

    Chamfering - roughing with 6mm 90 degree vee cutter

    Chamfering - finishing with 6mm 90 degree vee cutter

Slots and holes

    Roughing with 6mm end mill

    Finishing with 6mm end mill

    Chamfering - roughing with 6mm 90 degree vee cutter

    Chamfering - finishing with 6mm 90 degree vee cutter

Making amendments

The programs you can download using the above links were output from Vectric’s VCarve Pro program, but they have been edited to remove unwanted (and, in this case, unnecessary) tool change commands.

Take the Profile roughing program, fro example. Once a toolpath has been drawn and selected in VCarve Pro, the G Code needed to machine that path can be calculated and output by the built-in post-processor. That’s all fine, but because the post-processor tries to cater for all eventualities, the G Code program contains an initial tool change command. That’s annoying, because the program begins, then immediately pauses and asks for tool 1 to be inserted into the chuck. One easy way to deal with this is to edit the program using a word processor or text editor. The simple change is to remove a few lines of the program, near the beginning, like this:

Original first few lines of the program, showing the lines to be removed -

( Yamaha shield plate Pair profile 6mm AL endmill )

( File created: Friday, September 26, 2014 - 09:46 AM)

( for Mach2/3 from Vectric )

( Material Size)

( X= 210.000, Y= 120.000, Z= 4.000)

()

(Toolpaths used in this file:)

(Pair profile)

(Tools used in this file: )

(1 = End Mill {6 mm} Al)

G00G21G17G90G40G49G80

G71G91.1

T1M06

(End Mill {6 mm} Al)

G00G43Z20.000H1

S12000M03

(Toolpath:- Pair profile)

()

G94

Simply remove the lines shown above in red, and save the program. It works best if you save it with the same type of file extension as the original. I save my files with a text file extension (.txt) so it is easy to deal with them quickly in a text editor.

Note that the lines in this program are not numbered. The post-processor built into VCarve Pro and Cut2D inserts line numbers by default. I didn’t like that, so I used the facility in VCarve Pro to create a new post-processor, and simply removed the instruction to add line numbers.

Another annoying thing about the programs is that there is a very slow initial move from Safe Z (Z20) down to Z0. I can’t see the reason why it moves so slowly, but it is a real pain, as any move to safeZ is then followed by that same slow downward move to Z0. I chose to edit these programs to alter the first few lines, changing the sequence of moves to get to the initial X, Y, safeZ point, then inserted a faster feed rate (like F1000) to get to Z0.1 (i.e. just above Z0).

The message is that if you take reasonable care, you can customise the programs output by the post-processor, to suit your own purposes. That brings its own rewards, as well as its own risks, of course.

Article not yet available for download