powermill surface milling vs creo surface milling

Have you looked at the length of programs? Is powermill putting out IJK where creo is putting out point to point so its loading up your machine control speed?

Can you give more specifics on toolpath you created?  Is it Cutline Milling or Surface Milling and if so, which of the 3 options within Surface Milling? My initial thought is this has more to do with the post processor/controller unless you can see something strange when simulating the CL output within Creo even before you post process.

Not sure if anyone is still reading this thread 7 months later or not.  Oh, well.

I think the Powermill code outperforms the Creo code because of one line: G05.1 Q1.

It's towards the beginning of the Powermill code you shared.  What it basically does (to the best of my understanding) is this:

(Begin program - do all the G28/G17/G54 setup stuff)

G05.1 Q1

(Put the high-speed roughing code here)

G05.1 Q0

Basically, what your machine does when in G05.1 Q0 mode (which, I presume, would be the machine's default)

is:

1. Read line of code (G01 X-1. Y-1. Z1.)

2. Interpret -> GOTO X-1, Y-1, Z+1

3. Do the thing -> move the table

4. Check -> Am I at X-1, Y-1, Z+1?

5. Read next code

...and so on

Unfortunately, when you're trying to do "fast" stuff (ie, rough out a cavity), this method results in a jerky start-stop motion.

If you insert "G05.1 Q1" before the roughing cycle, the machine does:

1. Read code (G01 X-1. Y-1. Z1.)

2. Interpret -> GOTO X-1, Y-1, Z+1

3. Do the thing -> move the table

4. Read next code

In essence, the machine is speeding up the machining process by not constantly checking each and every position, or by not stopping after each move.  Different controls have different codes for controlling this motion (and different means of control - some change the gain in the servo drives, some change the "look ahead" (how many lines ahead of the current line the control reads to predict motion), some just turn off the "stop" effect after a motion).

Note: depending on your machine, you need to put the machine back in G05.1 Q0 mode before doing a canned cycle (drill, tap, etc.).

To insert the necessary code, you can:

1. (Easy but slightly inconvenient way) Just type it in.  Before you export each program to the machine, open your program in a basic text editor (e.g., Notepad) and insert the G05.1 Q1 line before your roughing sequences and G05.1 Q0 after them.  Save the file and post to the machine.  If you're handy with the machine control, you can also probably edit the file at the machine.

2. (Harder but more user-friendly way) Edit your post.  In your mfg assemby, select your workcenter and edit definition.  Look for the ID number of the post processor (for some reason, the workcenter in the file you shared has an ID of 1, but the none of the posts you shared are #1.  I think they are 12, 13, and 17).  Anyway, find the post your workcell is using (or should be using - and change the workcell to match!).  You can read the AustinNC documentation that came with Creo's post-processor (GPost).  Those documents will get you started in editing the post to get it to do what you want.

I hope this helps 😃

PS - I think the "R10" on that G05.1 Q1 line has something to do with the "fineness" of the high-speed control, but I'm not sure how it works.  Good luck!