5 axis help

[jmott]

I am looking to create a tool path to cut this 14° chamfer on the top of this part. Orange indicates what I am hoping to have the tool cut. I am looking to rotate the "A" axis to the 14° have the 1" endmill come down in Z and rotate about the "C" axis.

Machine is a Doosan VC630 5AX.

Any help would be appreciated.

Jason 

Mastercam2021

[Leon82]

That is going to leave a weird cup finish. Side mill it with old swarf

[cncappsjames]

Yeah, you can't machine that feature that way. If you want to Swarf it you need to make the floor your wall and the wall your floor.

[jmott]

Thank you guys for the the reply. It took a bit to get my head wrapped around the fact it would not cut this surface flat. I only have a level 2 mastercam license. Guess I will have to figure out another route to get this cut.

Jason 

[crazy^millman]

Should be able to rotate the A Axis to 104 degrees and side cut it. What is the Travel of the A Axis?

[Guest]

Just now, crazy^millman said:

Should be able to rotate the A Axis to 104 degrees and side cut it. What is the Travel of the A Axis?

In level 2 license?

[jmott]

I can reach but I am stuck with the level 2 license. unless you guys have a work around? 

 

[Guest]

Just now, jmott said:

I can reach but I am stuck with the level 2 license. unless you guys have a work around? 

 

I don't know if there is a better way, what I do if I have license limitations is drill a hole in the air aligned with the plane i want to machine, then drop the z axis and spin the c axis with a manual entry

(Drill or point toolpath in mastercam)

G1 z-.5 f5.

C360.

G0 Z10. .....

Maybe you could do it with a point toolpath and the toolpath editor

[crazy^millman]

1 hour ago, Thee Byte™ said:

I don't know if there is a better way, what I do if I have license limitations is drill a hole in the air aligned with the plane i want to machine, then drop the z axis and spin the c axis with a manual entry

(Drill or point toolpath in mastercam)

G1 z-.5 f5.

C360.

G0 Z10. .....

Maybe you could do it with a point toolpath and the toolpath editor

Kind of correct add a Cantext to your post to output C360. Then do a Contour toolpath with 2 lines meeting at the mid point use the toolpath editor to add that Cantext at the right place and you will get code to accomplish the task. I created a plane at the 104 deg angle to help get the B to kick over for this MMD.

Here is a .Z2G with this done and the post modifications I used to cheat this in.

Level 2 C360 Cheat

%
:0001(5TH AXIS)
(DATE=DD-MM-YY - 19-02-21 TIME=HH:MM - 12:31)
(MCX FILE - C:\USERS\RON\DOCUMENTS\MY MASTERCAM 2021\MASTERCAM\PARTS\5TH AXIS LEVEL 2 C AXIS CHEAT.MCAM)
(NC FILE - C:\USERS\RON\DOCUMENTS\MY MASTERCAM 2021\MASTERCAM\MILL\NC\5TH AXIS.NC)
(MATERIAL - ALUMINUM INCH - 2024)
(T1|HELICAL - 03662 - END MILL FOR ALUMINUM - 3 FLUTE X 45° HELIX X 0.7500 DIA X 1.6250 LOC X ZPLUS COATED |H1)
N100 G20
N102 G0 G17 G40 G80 G90 G94 G98
N104 G0 G28 G91 Z0.
N106 G0 G28 X0. Y0.
(HELICAL - 03662 - END MILL FOR ALUMINUM - 3 FLUTE X 45° HELIX X 0.7500 DIA X 1.6250 LOC X ZPLUS COATED |TOOL - 1|DIA. OFF. - 1|LEN. - 1|TOOL DIA. - .75)
N108 T1 M6
N110 G0 G54 G90 X1.7702 Y.85 C0. B-104. S10000 M3
N112 G43 H1 Z1.8221
N114 Z1.7721
N116 G1 Z1.5721 F150.
N118 X1.0202
N120 G3 X.2702 Y.1 J-.75
N122 G1 Y0.
N124 C360.
N126 Y-.1
N128 G3 X1.0202 Y-.85 I.75
N130 G1 X1.7702
N132 Z1.7721
N134 G0 Z1.8221
N136 M5
N138 G0 G28 G91 Z0.
N140 G0 G28 X0. Y0.
N142 G28 B0.
N144 M30
%

Here is the Post Mod. Remember to add the comment to the CANTEXT through the MMD/CMD.

pcant_out       #Canned text - build the string for output
      #Assign string select type outputs
      if cant_pos < three, #cant_pos indicates canned text output
        [
        if cantext$ = three, bld = one
        if cantext$ = four, bld = zero
        #Build the cantext string
        if cantext$ = one, strcantext = strcantext + sm00
        if cantext$ = two, strcantext = strcantext + sm01
        if cantext$ > four & cantext$ < 30, #Added Logic to support 4-29 Cantext output
          [
          strtextno = no2str(cantext$)
          strcantext = strcantext + strm + strtextno
          ]
        if cantext$ = 30, #Added for Level 2 C360. Cheat
           [
           pbld, n$, "C360.", e$
           ]
        ] 

Just some dumb guy who slept at a Holiday Inn Last night.

[Guest]

This is the manual entry thing I was saying. 

Would this not work?

Pocket Nc BAXIS ROT.mcam

It looks good in the Online Machine Simulator.

[Guest]

https://sim.pocketnc.com/

You could view the result with these files using the above link,

Pocket Nc BROT-STL.stl

Pocket Nc B-ROT.NC

[crazy^millman]

24 minutes ago, Thee Byte™ said:

This is the manual entry thing I was saying. 

Would this not work?

Pocket Nc BAXIS ROT.mcam

It looks good in the Online Machine Simulator.

Yes, but I provided a toolpath method that allowed them to control movement into and out of the cut. They could multi pass or depth of cut it what the CANTEXT process. The way you're coming up with requires a lot of fat fingering. The way I did only requires some toolpath editing and done.

14 minutes ago, Thee Byte™ said:

https://sim.pocketnc.com/

You could view the result with these files using the above link,

Pocket Nc BROT-STL.stl

Pocket Nc B-ROT.NC

Peter, sure that works? I see B120 and then B360. Wouldn't that only cover 240 degrees?

(DATE=DD-MM-YY - 19-02-21 TIME=HH:MM - 19:10)
(MATERIAL - ALUMINUM INCH - 2024)
(T1|POCKET NC TOOL 1/8 |H1)
N100 G20
N102 G0 G17 G40 G80 G90 G94 G98
N104 G0 G53 Z0.
N106 M9
N108 G49
N110 M5
N112 G0 G53 X2.5 Y2.5
(POCKET NC TOOL 1/8 |TOOL - 1|DIA. OFF. - 1|LEN. - 1|TOOL DIA. - .125)
N114 T1 M6
N116 G0 G54 G90 X0. Y1.371 B120. A27.849 S2139 M3
N118 G43 H1 Z1.9797
N120 S1000 M3
N122 G1 Z1.9297 F5.
N124 Z1.9797
G1 Z.9297 F5.
B360
G1 Z2.
N126 S2139 M3
N128 G0
N130 M5
N132 G1 Z1.9297
N134 Z1.9797
N136 G0 G53 Z0.
N138 M9
N140 G49
N142 M5
N144 G0 G53 X2.5 Y2.5
N146 G28 B0. A0.
N148 M30

 

[Guest]

41 minutes ago, crazy^millman said:

Peter, sure that works? I see B120 and then B360. Wouldn't that only cover 240 degrees?

Yes, you're right, I'll put a B0 before dropping the z in the manual entry.

B0.
G1 Z.9297 F5.
B360.
G1 Z2.

I like watching the table spin around anyway!

44 minutes ago, crazy^millman said:

Yes, but I provided a toolpath method that allowed them to control movement into and out of the cut. They could multi pass or depth of cut it what the CANTEXT process. The way you're coming up with requires a lot of fat fingering. The way I did only requires some toolpath editing and done.

Yeah, it sounds cool. I never do post edits tho, I leave that to the professionals for now..

I'm definitely going to try it Ron

[So not a Guru]

13 hours ago, Thee Byte™ said:

https://sim.pocketnc.com/

You could view the result with these files using the above link,

Pocket Nc BROT-STL.stl

Pocket Nc B-ROT.NC

That simulator is pretty sweet.

[Guest]

Just now, So not a Guru said:

That simulator is pretty sweet.

It really is!

When I started programming this, I was working on Mastercam Entry and it doesn't seem to support Machine Simulation.

All the operations had to be built in top Tplane and Cplane with different WCS, so you can't see the rotations in Mastercam.
 

The online Simulator makes it easy to spot if something needs improving!

[crazy^millman]

12 hours ago, Thee Byte™ said:

Yes, you're right, I'll put a B0 before dropping the z in the manual entry.

B0.
G1 Z.9297 F5.
B360.
G1 Z2.

I like watching the table spin around anyway!

Yeah, it sounds cool. I never do post edits tho, I leave that to the professionals for now..

I'm definitely going to try it Ron

I know a lot about post editing and can do a lot with them and leave it for the most part to the professionals. However this was one no one I know would show you since it allows someone to do 5 Axis work with a Level 2 Mastercam sim. Someone might get upset they are not getting a 5 Axis purchase. Nope if anything someone should see the value of getting a full 5 Axis seat because they are limited by not having it. When you have to hack a post and operations to get good code that is never a good thing, but sometimes we have to do what we have to do.

[Guest]

6 minutes ago, crazy^millman said:

I know a lot about post editing and can do a lot with them and leave it for the most part to the professionals. However this was one no one I know would show you since it allows someone to do 5 Axis work with a Level 2 Mastercam sim. Someone might get upset they are not getting a 5 Axis purchase. Nope if anything someone should see the value of getting a full 5 Axis seat because they are limited by not having it. When you have to hack a post and operations to get good code that is never a good thing, but sometimes we have to do what we have to do.

Lol, I would not call using Manual Entry or Canned Text a hack.

We could write our all our code in manual entry blocks if we wanted, but then we would never get anything done.

The Mastercam 5 Axis License lets you do your programs at blazing fast speed without the "fat fingering".

 

[Guest]

I saw Mastercam added optirough to Mill 2d in Mastercam 2022 beta which is so cool for all the users who have never tried it.

[cncappsjames]

4 hours ago, Thee Byte™ said:

Lol, I would not call using Manual Entry or Canned Text a hack.

Me either. I always prove out my probing cycles at the machine. Once proven, I put them in Manual Entries, and all is good and right in the world.

It's only a hack if you're trying to cheat the system. Things like this are precisely why Manual Entry was created, therefore, NOT a hack,

[Leon82]

3 hours ago, cncappsjames said:

Me either. I always prove out my probing cycles at the machine. Once proven, I put them in Manual Entries, and all is good and right in the world.

It's only a hack if you're trying to cheat the system. Things like this are precisely why Manual Entry was created, therefore, NOT a hack,

I use an NC program as text file.

 

Store in mastercam file.  It won't update of you repost it. But is immune from file path changes.

 

The other option. Reads file when posting so it's always up to date. Any filename or path changes will need to reselect the text file