null tool change problem

[nickz]

ok, this is strange! I am working between two fixture offsets G54 & G55. Facing one part at G54 and going over to face another at G55, (different heights). The output I get is missing the G54 machining code and goes over to G55 which has the code.

example:

N10M06T29( FACEMILL, 4.0" 45D FINISH)

M01

S2500M03

T12

G00G90G54P#550

X31.64Y145.

G43H29Z10.M08

G00G90G55P#550

(FACE TO 47.00MM THICK)

Y145.Z5.

G01Z.5F900.

Y-145.

G00Z10.

Y145.

Z5.

G01Z0.

Y-145.

G00Z10. <---- should be end of the G54 side

Y140.

Z8.

G01Z4.083

Y-140.

G00Z10.

Y140.

Z6.083

G01Z2.167

Y-140.

G00Z10.

Y140.

Z4.167

G01Z.25

Y-140.

G00Z10.

Y140.

Z2.25

G01Z0.

Y-140.

G00Z10.

M09

It seemed to combine both operations into one??? Can't force variables; pccdia or tloffno with an *, then the diameter offset number outputs on every single G1,G2, and G3 line.

 

[This message has been edited by nickz (edited 01-10-2001).]

[This message has been edited by nickz (edited 01-10-2001).]

[Allan Brown]

We call this a 'null toolchange' WCS issue. What version are you using? How is the WCS value set?

If you are using a pre-V7 era post with Misc Values (mi1) to change the wcs, you have to add logic to the ptlchg0 postblock, checking for a change in the mi1 variable.

[nickz]

Yes I am using the Misc Value (mi1) to change the wcs, don't know of any other way to do so. We are using Mill-V8, level 1. The post is MPYAS80M.PST, right off the V8 CD, with some minor mods that are not related to wcs. The controller is a Yasnac i80.

[Allan Brown]

The MPYAS80M post doesn't appear to handle this case well. The post does all kinds of buffering to output 2D contour codes for tangent or intersecting geometry (G201,G200,G199,G198).

You have a few options:

1) Force a tool change when switching the WCS within the same tool. From the operation's Tool Parameters page click "Change NCI..." then enable "Force tool change".

2) If you don't need the G201 type codes, switch to another standard G-Code post (Mpfan, Mpyasnak) and use the T/C plane Work offset method to switch your WCS.

3) Have your existing post edited to cover this scenrio. Contact your reseller.

4) As this is a default post, inform the CNC Software Post Dept. of the problem.

5) Hand edit your G-Code if this situation occurs rarely in your programming.

[nickz]

Thank you Dave,

I will probably start working on another post (MPYASNAK.PST) and will hand edit for now, when using old "default" post. I will also get in touch with both the reseller and CNC Software for lots of help.