Y Axis Machining

[Greg Williams]

Hi Guys,

 

We have a Sachman RP3 machine with a Heidenhian 422 controller, This machine has a universal head (the same deal as Huron, Correa and pacfic to name a few) With this machine like most bed mills the Z travel is greater that the Y travel so hence we do most of our machining on angle plates with the head rotated so that the Y axis is into the job (as in a horizoltal machine), Now to achieve the correct G code I have always done the following

1, drawn the job in the top veiw

2, do my toolpaths as normal

3, create a NCI file and rotate it 90 degress

4, Post that rotated NCI file

I do it this way because I first started using Mastercam with version 5 and that is how I did it back then.

Now with this being the year 2002 there must be a better way,

How do you folks do it?

 

PS I have V9 Level 3

[Allan Brown]

1. Draw your part as you do currently in the top and have your post rewritten to work out the rest.

 

2. Draw your part in the same orientation as it sits on the machine (easier on the brain I think), use Toolplanes in Mastercam, and again have your post rewritten to work out the rest.

[Greg Williams]

Thanks Dave,

 

I will have a go at editing my post, If I have no luck I will be in contact.

[GREG]

Greg

We just have a rotation of 0 at the start of the programe and rotation 0 at the end to cancel.Then the operators put in whatever is needed.

 

Cheers

[Greg Williams]

Greg,

 

When you say that you have a rotation at the start of the program, Do you mean the Canned cycle rotation that is found in all Heidenhain's (The cycle number I Can't remember) or the 3D rotation that is found on the 426 controller

[GREG]

Greg

This is the start and end sequence we use.

0 BEGIN PGM TEST MM

1 ; PROGRAM NAME - T

2 ; DATE-22-03-02 TIME-13:31

3 ; 10MM ENDMILL ROUGH

4 TOOL CALL 1 Z S15000

5 CYCL DEF 7.0 DATUM SHIFT

6 CYCL DEF 7.1 # 0

7 L B+0 C+0 R0 F MAX

8 CYCL DEF 10.0 ROTATION

9 CYCL DEF 10.1 ROT 0

 

16 L Z+100 R0 F MAX

17 CYCL DEF 7.0 DATUM SHIFT

18 CYCL DEF 7.1 # 0

19 CYCL DEF 10.0 ROTATION

20 CYCL DEF 10.1 ROT 0

21 M05

99999 END PGM TEST MM

 

Cheers

[Christian Raebild]

Cycle 10 rotates around the Z axis, and can be found on most Heidenhain controls. Cycle 19 creates a new toolplane (any orientation), but is only found on newer TNC 426/439 controls and the iTNC 530 control