cancel
Showing results for 
Search instead for 
Did you mean: 
Security Alert Log4j Security Vulnerability. Click here to know more.
cancel
Showing results for 
Search instead for 
Did you mean: 

powermill surface milling vs creo surface milling

asifcad
12-Amethyst

powermill surface milling vs creo surface milling



see these videos both videos shown surface machining on same surface one is from power mill other is from creo parametric...in creo machining there is some motion pause during one patch to other patch of surface ..but in power mill no pause continue machining ..why this is happening...is it software capabilities issue or i am some thing missing..please advise..

 

fisa

17 REPLIES 17
Todd_Reiter
4-Participant
(To:asifcad)

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?

i check it there is no IJK value in power mill gcode please check attach file ..you can run this file on cimco edit.

 

regards

 

asif

 

 

please check attachment for compare both g codes

 

 

bnguyen-2
6-Contributor
(To:asifcad)

Hi

please please check post form powermill if z=-10 total lengh =32.200 lines, in Creo NC z=-10 total lengh =2.940 lines that meaning post in PowerMill tolerance more 10 time compare with Creo NC.

Your problem is using default post in Creo, you should edit post processor in Creo more tolerance

compare post powermill.JPG

Todd_Reiter
4-Participant
(To:asifcad)

 

Disregard that responds, I looked at the line numbers wrong.

i already increase the tolerance but no change also insert this command for look ahead option enabled but no change ...some one say me that change your software ...power mill more advance  software compare to creo ..but my heart is not accepting this .

 

 

Todd_Reiter
4-Participant
(To:asifcad)

Sad to say they might be correct.  We use power mill for our robots and Creo for our CNC machines and we are transitioning into more of the 3D tool modeling and true 5 axis milling in creo. Sadly on the daily I am becoming less and less impressed with creo.

bnguyen-2
6-Contributor
(To:Todd_Reiter)

Dear 

Take a look for technical side: Post processor is important please work with who sold Creo for you to got support.

Do you check to compare why? you are sure same as bellow

- NC code same: example in Creo have N1000 X-041.644 Y012.064 Z-005.886 maybe machine run different with non N...

- With kind of tool path using in Power Mill? then Creo using toolpath same with kind this tool path

- Make NC same surface, step depth, step over...

- change any thing same NC code, much be have some differnce

Ask? why x,y,x,F same... but machine run not same? 

If to clear that work with who support then test above you will got ideas

I dont have your code, your machine CNC I cant filling and support

Tks

bnguyen-2
6-Contributor
(To:asifcad)

Dear

I had fond a Problem that many small arc G3 in Creo NC code that why machine pause at that position

In Powermill NC code only G1 dont have G3

***for some case 3D ARC dont export nc code G2 G3 set in Creo only G1 or you make post processor G01 only

Open you  Creo NC , Powermill nc code in Cimco edit you will see

For Technical you must to check it, can not said that software... 

Problem nc code mall G3.JPG

 

asifcad
12-Amethyst
(To:bnguyen-2)

ok bro i send you my mfg file and pp from which i generate code..may be this can you help understand better.because i do all the thing where all of you point me.i am still sure that creo have all the nc capabilities like other high end and cost software

 

 

bnguyen-2
6-Contributor
(To:asifcad)

Hi

If your are PTC's customer please contact PTC support

I dont have your machine I cant take time for this case.I can do for you but it will take a long discussing

I see you model copy surface from other part maybe model tolerance, Can you design other part with same revolve then using cutline with points.

Alot customer using Creo NC but no comment about this.

TKS

slolli
5-Regular Member
(To:asifcad)

I took a quick look and just a few things to consider:

  1. Your tolerance in the toolpath is .0001 while your model accuracy is approximately .0018. You never really want tolerance in a sequence tighter than accuracy on the model.
  2. I wonder if your post processor is setup to handle the parameter HELICAL_CIRC_INTERPOLATION a different way than the post that is handling powermill.  Yours is set to HELICAL_CIRC_INTERPOLATION = POINTS_ONLY so it is spitting out tons of GOTO moves, will your post handle ARC moves?
asifcad
12-Amethyst
(To:slolli)

you means that sequence accuracy must be same as model accuracy ??

 

which option you suggest for HELICAL_CIRC_INTERPOLATION??

slolli
5-Regular Member
(To:asifcad)

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!

sir really sorry for the late reply ..and thanks for the detailed explanation. now its time to follow your instruction

 

regards

 

Asif

Announcements