How to copy toolpath(s) from G54 to G55 in Mastercam

[PGcam]

Tutorial: Simplest method for copying toolpaths to G55 in Mastercam and avoiding manual gcode editing

I’ve encountered several CNC programmers who aren’t familiar with the use of planes in Mastercam, even with years of experience, so I decided to make this tutorial. Hopefully it’s easy and intuitive to follow.

This is the quickest way to duplicate your toolpaths to your 2^nd part in another vise in your machine, once you get the hang of the steps in the procedure.

This method eliminates unnecessary tool changes, and if you make changes in the source toolpath, they will automatically be applied to the transformed toolpath copy. Making production faster and more efficient, even if you have to edit your program in Mastercam later.

 

Let’s begin…

 

STEP 1

First, model and toolpath your 1^st part.

 

 

STEP 2

Translate-copy your model somewhere to the side, in X or Y direction. Distance doesn’t matter but avoid changing Z height, to keep the process simple.

Now you have 2 models at some random distance appart. One will be your G54 and the other your G55.

At the end, Mastercam will output G54 for your Top plane, and G55 for the other plane we’re about to make.

The two different points is where you will pickup with your edge-finder while setting up your two parts for simultaneous machinning.

The terms Plane, Program Origin, Offset, Pickup Location, G54, G55, G56, etc…  all mean the same thing in this case.

 

 

STEP 3

After copying your model to the side…

Go to the Planes manager panel, right-click on the plane you’re using for your 1^st part (TOP?), select Duplicate

Normally when you duplicate the "Top" plane, it will show up as "Top-1", this is what you want to Edit (move and rename). In my screenshot I already have it renamed. Terrible, I know...

Edit the duplicate plane: shift it to the same location on the 2^nd part, give it a new name like “Top @ G55”, or “Origin 2”, whatever you want to name it, accept changes.

 

 

STEP 4

Now go to your Toolpaths tab, click on Toolpaths Transform

 

STEP 5

In the Transform Operation Parameters window, make sure to select:

Source operation: your source toolpath

Type: Translate

Method: Tool plane; checkmark Include Origin

Source: Geometry

Group NCI output by: Operation type

In Comment box write: “TRANSFORM TO G55”; this will add a separate line of text on top of existing toolpath name in final NC output, to make it easier to differentiate between source toolpath and a transformed toolpath

 

In the same Transform Operation Parameters window, now go to the next tab Translate, and select the following:

Method: Between planes

Checkmark: From plane; select part 1 origin

To plane: select part 2 origin (the plane you duplicated and moved)

Under Pattern origin shift: click on the mouse cursor button under From part, select origin 1 location

Under Pattern origin shift: click on the mouse cursor button under To part, select origin 2 location

 

 

END RESULT

Nice clean NC (gcode) output, with automatic G55 output, no unnecessary toolchange or send-to-home commands.

When tool is done machining 1st part @ G54, it rapids to the clearance plane Z2., and goes directly to machine your 2nd part @ G55 without any interruption.

 

 

If for any reason you DO want to send-tool-home and M01 between your source toolpath and tansformed toolpath (if for example, you’re proving your 1^st part before running production), you can always checkmark the “Force tool change” option, and turn it off after you’ve proven your program, to speed up production.

 

Hope this useful to someone out there in the beginning of their programming career.

If you’re doing this for the first time, it may take a while to practice and understand the steps, but once you get used to it – you're on autopilot. It takes only a minute to get a toolpath transform.

If you already know all this, excellent! Please share some other useful tips on this topic.

-          Paul G.

[Leon82]

You don't have to make a duplicate plane. You can assign a new offset per instance and keep the offset distance at zero.

[SuperHoneyBadger]

Keeping the same planes with a 0 in all fields for offset deltas gives you the ability to do n copies instead of one per physical (virtual?) plane, as per above post. And you can verify all copies of your toolpaths on a single original solid, including 2nd ops.

It can get hairy moving and copying, especially for the next guy who has to open your programs later. Source: am next guy opening old programs.

[PGcam]

6 hours ago, Leon82 said:

assign a new offset per instance and keep the offset distance at zero.

Leon, would you mind posting some screenshots of what you're referring to?

[Leon82]

[jpatry]

6 hours ago, Leon82 said:

Yes, my main co-conspirator introduced me to this method, it works magnificently

[PGcam]

On 9/11/2023 at 10:16 AM, Leon82 said:

Leon, in my original post I describe how to get the same toolpath @ G54 and G55.

From your screenshots, all I get is duplicate gcode @ G55. G54 does not even generate.

What am I missing?

[Leon82]

put the increment at one also

 

[PGcam]

I still get same result as in my previous screenshot. 

Weird.

I really want to see it work, but must be doing something dumb.

[crazy^millman]

13 minutes ago, PGcam said:

I still get same result as in my previous screenshot. 

Weird.

I really want to see it work, but must be doing something dumb.

Can you share a sample file with your post to see if it is post related?

[Werktuigbouwer]

Also set the start field to 0

And delta to 2

[crazy^millman]

6 hours ago, PGcam said:

Yes, please take a look:

BIIG MORI SEIKI - PAUL G'S CUSTOM MACHINE POST.pst 93.4 kB · 1 download

Need that sample file.

[PGcam]

1 hour ago, crazy^millman said:

Need that sample file.

What's the extension and the usual location of that file?

[PGcam]

6 hours ago, Werktuigbouwer said:

Also set the start field to 0

And delta to 2

2 Instances?

or Click +1 & +2 buttons and draw a line?

Or set some other value under the Translate tab?

 

I've tried a bunch of combinations. The closest I get is G54 and G55 output, but now get extra duplicate code under G54.

[crazy^millman]

1 hour ago, PGcam said:

What's the extension and the usual location of that file?

.mcam a Mastercam file or a .z2g or .mcam-content

[PGcam]

7 minutes ago, crazy^millman said:

.mcam a Mastercam file or a .z2g or .mcam-content

Oh sorry, didn't know what you meant by "sample file". 

Are you able to open .mcam from Mastercam 2022?

[crazy^millman]

1 hour ago, PGcam said:

Oh sorry, didn't know what you meant by "sample file". 

Are you able to open .mcam from Mastercam 2022?

Yes I that is far back as I go on my 1st drive. I have until 2018 on my 2nd bootable drive. I am running a dual boot system where I can go back in time so speak without having to have it all on one drive. 

[Werktuigbouwer]

6 hours ago, PGcam said:

2 Instances?

or Click +1 & +2 buttons and draw a line?

Or set some other value under the Translate tab?

 

I've tried a bunch of combinations. The closest I get is G54 and G55 output, but now get extra duplicate code under G54.

In start field:

0 = G54

Increment field to 1, so when delta = 2 you would get output for G54 and G55

[PGcam]

5 hours ago, Werktuigbouwer said:

In start field:

0 = G54

Increment field to 1, so when delta = 2 you would get output for G54 and G55

How do you set delta = 2?

[Johnward Holmeson]

On 9/16/2023 at 4:50 AM, PGcam said:

How do you set delta = 2?

Instances 2 is what he means I believe.