Product Levels

[gcode]

28 minutes ago, jeff said:

That's not on the default 3D license, is it? Or are you saying that I can add some multiaxis toolpaths individually?

Yes.. I believe there are a couple on mutilaxis toolpaths that can be added to a 3D license without buying the full mutiaxis module.

It's been a couple of years since that came up and may have changed since then.

[Newbeeee™]

34 minutes ago, gcode said:

Yes.. I believe there are a couple on mutilaxis toolpaths that can be added to a 3D license without buying the full mutiaxis module.

It's been a couple of years since that came up and may have changed since then.

We have curve/drill 5ax on our level 3 licence.

[Jayson Kramer]

1 hour ago, gcode said:

Yes.. I believe there are a couple on mutilaxis toolpaths that can be added to a 3D license without buying the full mutiaxis module.

It's been a couple of years since that came up and may have changed since then.

Gcode the options are still there instead buying a whole multiaxis. but getting the Multiaxis really does give some other tools not just for doing 5axis as you know.

[gcode]

52 minutes ago, Jay Kramer @ Precision Programming said:

Gcode the options are still there instead buying a whole multiaxis. but getting the Multiaxis really does give some other tools not just for doing 5axis as you know.

I had Mill Level 3 back in v9 days so I got grandfathered into multiaxis when they added  that module

I can't imagine a seat of Mastercam without miltiaxis

[Newbeeee™]

5 hours ago, gcode said:

I can't imagine a seat of Mastercam without miltiaxis

It's a slog...

[jeff]

13 hours ago, Jay Kramer @ Precision Programming said:

Gcode the options are still there instead buying a whole multiaxis. but getting the Multiaxis really does give some other tools not just for doing 5axis as you know.

We only have 3 and 4 axis machines. How many of the 5 axis toolpaths would be beneficial to me?

[Guest]

23 minutes ago, jeff said:

We only have 3 and 4 axis machines. How many of the 5 axis toolpaths would be beneficial to me?

Many but not all......many of them can be locked to 3 & 4 axis...some offer some pretty nifty options but other than 5 AX Drill & 5 Axis curve, you cannot pick and choose, it's all or nothing

Edited May 25, 2017 by Guest

[gcode]

4 hours ago, jeff said:

We only have 3 and 4 axis machines. How many of the 5 axis toolpaths would be beneficial to me?

I use 5X drill for rotary drilling on HBM's daily

Typically you'd use a toolplanes to define the rotations and you get one canned cycle per rotation

If the angles are even you can use Transfom/Rotate for the rest of the holes.. if they are not, you're building tool planes

and more drilling ops

With 5X drill you can do multiple holes at multiple uneven angles with one tool path

and your output is one canned cycle and a  positional line for each hole

This code was generated by one 5X tool path with a 4X HMC post

N100 ( 1"-X-120-DEGREE-SPOT-DRILL-3"-OOH   )
( *** G55 B90 *** )
( SPOT-CHECK-OD-HOLES )

T1 M6
M01

G0 G54 G17 G90 X2.72 Y0. C65. B90. W0. S1500 M3
M10
G43 H1 Z28.
G81 G98 Z20.169 R20.279 F5.
X.95
C185.
X2.72
C305.
X.95
G80
M5
G0 G28 G91 Z0. W0.
M01

With a 3D license and tool planes it would take  a drilling op and a translation/rotate OP

The  output would be 3  separate canned cycles

 

correction ...  this was done with a 5X post..  but a 4X post will work just as well with drill paths rotating about the B axis

[jeff]

Sounds like I need to tell my boss to get it.  

[Jayson Kramer]

2 hours ago, gcode said:

I use 5X drill for rotary drilling on HBM's daily

Typically you'd use a toolplanes to define the rotations and you get one canned cycle per rotation

If the angles are even you can use Transfom/Rotate for the rest of the holes.. if they are not, you're building tool planes

and more drilling ops

With 5X drill you can do multiple holes at multiple uneven angles with one tool path

and your output is one canned cycle and a  positional line for each hole

This code was generated by one 5X tool path with a 4X HMC post

N100 ( 1"-X-120-DEGREE-SPOT-DRILL-3"-OOH   )
( *** G55 B90 *** )
( SPOT-CHECK-OD-HOLES )

T1 M6
M01

G0 G54 G17 G90 X2.72 Y0. C65. B90. W0. S1500 M3
M10
G43 H1 Z28.
G81 G98 Z20.169 R20.279 F5.
X.95
C185.
X2.72
C305.
X.95
G80
M5
G0 G28 G91 Z0. W0.
M01

With a 3D license and tool planes it would take  a drilling op and a translation/rotate OP

The  output would be 3  separate canned cycles

So Gcode you never just on a 4th axis drill just create points at the top of the holes and do Drill standard and select window points to drill all and set to Axis on the rotary and be done?

 

[gcode]

1 minute ago, Jay Kramer @ Precision Programming said:

So Gcode you never just on a 4th axis drill just create points at the top of the holes and do Drill standard and select window points to drill all and set to Axis on the rotary and be done?

 

no. I've never tried that ... but I will

[Jayson Kramer]

4 hours ago, jeff said:

We only have 3 and 4 axis machines. How many of the 5 axis toolpaths would be beneficial to me?

Did you see the answer from John. alot of the paths have options for 4th. Also if you want to do full 4th work and not axis sub you need the multi axis using the 5th axis paths to get 4th output.

Just now, gcode said:

no. I've never tried that ... but I will

Do you want a sample I use for training?

 

[Jayson Kramer]

Looks like this.

[taperlength]

What happens if a file done on Mill 3D is opened on a computer with only Mill ?

[Jayson Kramer]

Just now, taperlength said:

What happens if a file done on Mill 3D is opened on a computer with only Mill ?

you will see all the paths and you can review them and backplot and so on. but if there is a surface toolpath with multi surfaces you will not be able to modify it.

 

[gcode]

21 minutes ago, Jay Kramer @ Precision Programming said:

Looks like this.

what does the posted code look like

[Jayson Kramer]

Gcode here:
O0
(AXIS SUB)
(DATE=DD-MM-YY - 25-05-17 TIME=HH:MM - 09:19)
(MCX FILE - C:\USERS\JKRAMER\DESKTOP\AXIS SUB.MCAM)
(NC FILE - C:\USERS\JKRAMER\DOCUMENTS\MY MCAM2017\MILL\NC\AXIS SUB.NC)
(MATERIAL - ALUMINUM INCH - 2024)
(T1|1/4 DRILL COBOLT EXT1.|H1|D1|TOOL DIA. - .25)
N100 G20
N110 G0 G17 G40 G49 G80 G90
(DRILLING USING ROTARY AXIS POSTIONING)
N120 T1 M6
N130 G0 G90 G54 X-13. Y0. A80.14 S1833 M3
N140 G43 H1 Z13.
N150 M8
N160 G98 G83 Z4.9149 R6.25 Q.1 F14.7
N170 X-11.5556 A40.14
N180 X-10.1111 A-.14
N190 X-8.6667 A-39.86
N200 X-7.2222 A-80.14
N210 X-2.8889 A-159.86
N220 X-1.4444 A-200.14
N230 X-2.8889 A-239.86
N240 X-10.1111 A-240.14
N250 X-13. A-239.86
N260 G80
N270 M5
N280 G91 G28 Z0. M9
N290 G28 X0. Y0. A0.
N300 M30
%

[gcode]

Cool.. that's the nice thing about MC, multiple  ways to do the same thing

[Jayson Kramer]

Here is the file with samples of few of the Axis sub options and even Drill 5 axis. most you know.

Axis Sub.mcam

[jeff]

3 hours ago, Jay Kramer @ Precision Programming said:

Did you see the answer from John. alot of the paths have options for 4th. Also if you want to do full 4th work and not axis sub you need the multi axis using the 5th axis paths to get 4th output.

 

 

Yes I saw that. I'm really leaning towards getting the Curve/5ax Drill add on

[Jayson Kramer]

2 hours ago, jeff said:

Yes I saw that. I'm really leaning towards getting the Curve/5ax Drill add on

I guess the question is what are you going to do with it . are you trimmng edges on a 5axis router for example?

[jeff]

14 hours ago, Jay Kramer @ Precision Programming said:

I guess the question is what are you going to do with it . are you trimmng edges on a 5axis router for example?

We get jobs on occasion where I need to cut profiles on my 4th. And it's a real p.i.t.a. for me to do it now. Am I wrong in thinking that the curve toolpath would help me?

We don't have 5 axis capability.

[crazy^millman]

18 minutes ago, jeff said:

We get jobs on occasion where I need to cut profiles on my 4th. And it's a real p.i.t.a. for me to do it now. Am I wrong in thinking that the curve toolpath would help me?

We don't have 5 axis capability.

A lot of the 5 Axis Toolpaths would help you here.  Many can be locked to just 4 Axis output. I did that for years by hand and I can do in 30 minutes what use to take me 120 hours to do by hand using Mastercam.

[Matt@ShopWare]

We did a webinar on using 5x toolpaths for 3x applications recently. Should be helpful for some of the discussion here. 

 

[Jayson Kramer]

Nice job Matt Thanks for sharing.