4 -axis toolpath?

[Stebedeff]

Maybe a stupid question. Is it possible to make a flow 5 axis or curve 5-axis toolpath without using the corde height or step increment. I'am testing/learning myself. What I want to do is just mill a round axle with a ballnose using my 4th axis. For example: If I would program by hand it would look like this for a 1" axle. WCS is the center of the axle.

G00 X0. Y0. Z1.5
G01 Z0.5
H360. ( INCREMETN 4TH AXIS 360 DEGREES TURN )
X0.1
H360.
X0.2
H360.
etc. etc.

I'am wondering how to do this in mastercam. Right now I get threw with the 5axis toolpaths but the corde height or step increment are my trouble. They just generate to much lines unnecesary.
Just testing....

Greetings

[Khalid]

I don't know Mastercam but the guy here has a good experience of 4th axis indexing...
Diy- Build Router In 10 Days
Diy- Build Router In 10 Days

[Stebedeff]

Thanks for your help Khalid. But this is not helping me. Sorry.
The thing is that I do use 4th axis toolpaths and get quit good results. But this seems just too easy for mastercam or something. It's not for a job or anything. It's to push myself learning and understanding mastercam. I think of stuff that I never dealt with and try to get it done. But right now I aint getting it done. So any help would be kind. BTW I'am using X3.

Greetings

[tstom]

Use flow5axis locked to 4 axis out put for tool control use "to a point" put a point at the center of your axle and pick that after you click the "to point "radio button
that will keep your y axis locked on center


If this isn't what you want post your file and we'll figure something out

Thought about this some more .....you could also use contour with axis substitution if you don't want to use sufaces to drive the tool

[cadcam]

Here is a simple 1/8 ball around a 1" dia. using axis sub . just a 1" arc used.

%
O0000
(PROGRAM NAME - T )
(DATE=DD-MM-YY - 11-04-09 TIME=HH:MM - 10:35 )
N100 G20
N102 G0 G17 G40 G49 G80 G90
( 1/8 BALL ENDMILL TOOL - 249 DIA. OFF. - 249 LEN. - 249 DIA. - .125 )
N104 T249 M6
N106 G0 G90 G54 X0. Y0. A-90. S4278 M3
N108 G43 H249 Z1.5
N110 Z.6
N112 G1 Z.45 F6.16
N114 A-450. F784.43
N116 G0 Z1.5
N118 M5
N120 G91 G28 Z0.
N122 G28 X0. Y0. A0.
N124 M30

[cob]

this might not be deeling with this question .
but I have a question on this post after G43 I knowctice your the post also posted H249. Can you please explain to me what the difference is when it post the tool number and I also knowtice sometimes it will post G43 H0.
What is the right way.
thanks


N104 T249 M6
N106 G0 G90 G54 X0. Y0. A-90. S4278 M3
N108 G43 H249

[Superman]

Good question

CAD / CAM programmers general rule of thumb
When they assign a # to a certain tool, they will make the tool length and Radius offset numbers the same

Tool #1 will have the lenth offset =H#1 as well as the compensation radius =R#1

OK, some machines have the length called up at toolchange and do not actually call-up the offset

cadcam's example
( 1/8 BALL ENDMILL TOOL - 249 DIA. OFF. - 249 LEN. - 249 DIA. - .125 )
- tool header has T249 H249 and D249 using 1/8" Ballnose

using H0 or a D0 in a program is not good practice, it is cancelling any compensation that was previously set

eg
G43 H249 Z0. ( spindle goes to Z0, but stands off by the value in H249 )

G43 H0 Z0. ( spindle goes to Z0, cancel any length comp. ) ( DANGER) (with or without a tool in the spindle )

G43 H249 ( length compensation taken up by the value in H249--- no machine movement )

Getting a H0 or a D0 , the tool setting page has not been set-up completely,
or the .MMD is not set to take the tool #s into the offset #s area automatically

[cob]

thanks for the reply.
so let me get these staight, after G43 the H# has to be the same as the tool number no matter what. and also the dia offset has to be 1


( 1/8 BALL ENDMILL TOOL - 249 DIA. OFF. - 249 LEN. - 249 DIA. - .125 )
- tool header has T249 H249 and D249 using 1/8" Ballnose

For this example do you mean on the (TOOLPATH PARAREMETER PAGE)
tool name =1/8 endmill

TOOL# =1 Len.offset= 1
Head #=1 Dia.offset= 1

is this the way it should be on the parameter page when ever I pick a tool.

[Superman]

after G43 the H# has to be the same as the tool number no matter what. and also the dia offset has to be 1.

Yes, you are setting up a proceedure, the operator would expect the tool length and radius comp to be under the same number as the tool.

( 1/8 BALL ENDMILL TOOL - 249 DIA. OFF. - 249 LEN. - 249 DIA. - .125 )
- tool header has T249 H249 and D249 using 1/8" Ballnose

For this example do you mean on the (TOOLPATH PARAREMETER PAGE)
tool name =1/8 endmill

TOOL# =1 Len.offset= 1
Head #=1 Dia.offset= 1

is this the way it should be on the parameter page when ever I pick a tool.

If you set the tool up correctly on the tool parameter page, spindle RPM, coolant, feeds, tool description, etc. when you select another operation with this tool, all data will go with it.

When you create a new tool, and assign a tool # to this tool, the length offset and diameter offset #s should also update to the # assigned to the tool. ( This is rectified in the .MMD file )

BTW - Head # is not a critical item, it may be used for special custom set-ups, double columns, mill-turns, lathes. It can be left at it's default setting of (-1).

[cob]

sorry for taking this tread out of contents.
but THANK YOU SUPERMAN
for explaing this set up thing .
know I just have to figure out where to do all the modification for my post.
thanks again

[Stebedeff]

Thanks cadcam! But how to do it with steps of 0.1 or whatever without the retract? It does work with multipass. But keeps retracting. I would like to have it looking like this .....

G00 G43 H1 Z0.5
G01 Z0.0 F500
X0.0
U360.0
X0.1
U360.0
etc.
etc.

Thanks to all.....

[kiemkhach]

Message edited