Hello Guest it is November 19, 2019, 04:06:42 PM

Author Topic: Questions 1st Aluminum Cut Sample  (Read 8912 times)

0 Members and 1 Guest are viewing this topic.

Offline kolias

*
  •  1,011 1,011
    • View Profile
Re: Questions 1st Aluminum Cut Sample
« Reply #20 on: November 13, 2012, 01:31:04 PM »
The results today were perfect as per attached pic and next time I will use even a slower feed rate

Used a feed rate of 10"/min and about 8000RPM for both the square cutout and the engraving.

The cutout was with an 1/8" 2 flute carbide end mill and the engraving with 1/8" V engraving carbide end mill.

Cutting the square I notice that when the tool plunged to the surface was a rough plunge but did a nice job anyway.

Is there a difference between the tool I used to cut the square and a center cutting end mill ?

On the picture I have from a catalogue they both look the same
Nicolas

Offline Fastest1

*
  •  927 927
  • Houston, TX
    • View Profile
Re: Questions 1st Aluminum Cut Sample
« Reply #21 on: November 13, 2012, 07:45:18 PM »
The lower picture looks like a 2 flute end mill, hard to say if it is center cutting however plunging is an aggressive move and on my machines I generally get uncomfortable and flex or deflection seems visible during the action but I dont see it in the results. It might just be paranoia on my part. You might try slowing the plunge rate of that tool, not the feed rate. Otherwise everything looks great. And congrats. Also think twice about slowing the feed down and confirm it in the feed and speeds calculator if possible.
I want to die in my sleep like my grandfather, not like the passengers in the car! :-)

Offline ger21

*
  • *
  •  6,288 6,288
    • View Profile
    • The CNC Woodworker
Re: Questions 1st Aluminum Cut Sample
« Reply #22 on: November 13, 2012, 08:00:18 PM »
Don't plunge, ramp into the cut.
Gerry

2010 Screenset
http://www.thecncwoodworker.com/2010.html

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html

Offline kolias

*
  •  1,011 1,011
    • View Profile
Re: Questions 1st Aluminum Cut Sample
« Reply #23 on: November 13, 2012, 09:14:25 PM »
Fatest1 you are right, it is just a 2 flute end mill and not a center cutting. I just ordered one 2 flute center cutting and one 4 flute center cutting and I'm anxious to try them. Your idea about slowing the plunge from 15"/min I have now sound good but why you say not the feed rate?

I was thinking to get the feed rate down to 7"/min

Gerry its no problem to ramp into the cut on the samples I do now but when I do the cut of my control panel (see panel picture above) I will not be able to do that because It will not be nice to see the ramp on the finish product (I assume by ramp into the cut you mean Lead-in) 
Nicolas

Offline ger21

*
  • *
  •  6,288 6,288
    • View Profile
    • The CNC Woodworker
Re: Questions 1st Aluminum Cut Sample
« Reply #24 on: November 13, 2012, 09:31:17 PM »
No, not lead in. You ramp down to the depth, rather than plunge. Start at the surface and gradually move down while following the toolpath. Say your cutting your square shape. Start at the corner, at the surface. While moving along the first side, ramp down to the final depth, then go all the way around and go over the ramped portion to bring it to the full depth.
Gerry

2010 Screenset
http://www.thecncwoodworker.com/2010.html

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html

Offline Fastest1

*
  •  927 927
  • Houston, TX
    • View Profile
Re: Questions 1st Aluminum Cut Sample
« Reply #25 on: November 13, 2012, 09:39:26 PM »
I could never plunge at 15" a minute with an end mill (not in my present configuration anyway). I would most likely plunge in the 3-4 inch per minute range but I am conservative when breaking tools (that was a joke) my feed rates might be in the 10-16 ipm though I am limited by a 1900 rpm ceiling at the moment. Also as Gerry mentions and I recommended you practice on some scrap, ramping is a form of entry and should leave no marks that arent removed with a finish pass. The helical ramp if used would have been used on the inside of the square, again only noticeable if the small square piece is the part you are keeping. I believe you are trying to cut the panel and the square would be scrap. Same for ramping in along/parallel to your line of cut, the tool should be cutting not dragging and therefore deflecting off path. I only mentioned the feed rate becasue you should stick to what the calculated feed is for that tool and conditions.
« Last Edit: November 13, 2012, 09:41:16 PM by Fastest1 »
I want to die in my sleep like my grandfather, not like the passengers in the car! :-)

Offline kolias

*
  •  1,011 1,011
    • View Profile
Re: Questions 1st Aluminum Cut Sample
« Reply #26 on: November 13, 2012, 09:46:33 PM »
Not sure what you mean Gerry. For the square, the material is 1/8" thick and I did 4 passes each 0.03125 and the engraving total depth is 1/16" and I did it in 2 passes of 0.03125 each

Otherwise how can I gradually move down? MastercamX5 does not have something like that as far as I know (which is not very much lol)

Fastest I like the 3-4" plunge and I will do it and yes the squares I cut are scrap
Nicolas

Offline Fastest1

*
  •  927 927
  • Houston, TX
    • View Profile
Re: Questions 1st Aluminum Cut Sample
« Reply #27 on: November 13, 2012, 10:55:06 PM »
The lead in will allow you to do just as Gerry is suggesting. I am sure MC has these same abilities if not more. You are running a higher rpm than I can IIRC 8000rpm? so your plunges could be faster than mine but just try to get to depth first and then let the side of the tool do the cutting. When I say square, the cutout that will be scrap (the part right above the word "spindle") could be where the entry was initiated or ramped in parallel a s Ger is saying. Do you ever simulate it, or run it in Mach with the tool above the work or the machine off but running Mach? I do this sometimes due to ignorance of the proper way to a simulation or verify.
I want to die in my sleep like my grandfather, not like the passengers in the car! :-)

Offline kolias

*
  •  1,011 1,011
    • View Profile
Re: Questions 1st Aluminum Cut Sample
« Reply #28 on: November 14, 2012, 12:06:04 AM »
But Gerry said is not the Lead-in but "gradually move down while following the toolpath" and this I dont know how to do it. Maybe there is a command doing this but I'm now aware of it.

Also I dont know how to define the entry of the tool inside the square (scrap) as you say Fastest1. I select all my squares I want to cut and Mastercam picks a corner on each and does the rest. Dont forget that its not one square to be cut in my control panel so I dont see how this can be done.

I do simulate the cut in Mastercam to assure that all is ok before I get the gcode to Mach3.
Nicolas

Offline RICH

*
  • *
  •  7,371 7,371
    • View Profile
Re: Questions 1st Aluminum Cut Sample
« Reply #29 on: November 14, 2012, 06:20:57 AM »
You could change a few lines of code if your program does't provide for ramping into the material. ie;

G01 Z-........ F.....
G01 X ........ F......

To

G01 Z-.......X.......F....
Which will provide for ramping into the material

RICH