POST HELP

[DavidB]

With this multi pass 2d contour toolpath I'm getting a Y Z move on the same line which is not correct.

What post mod can I make to get a Z move before the Y axis feed move?

Here is a snippet of the posted G-code .....

 

T8 M6 pcomment$ p_goto_strt_tl 70.

G00 G54 G90 X-422.455 Y-45.5 A90. B90. S640 M03 pcomment$ p__5:879 70.

M12 pcomment$ p__6:887 70.

M10 pcomment$ p__6:887 70.

G43 H8 Z73.991 pcomment$ p__3:870 70.

M08 pcomment$ p__3:870 70.

Z33.841 prapid$ prapidout 72.

G01 Y-23.5 F230. plin$ plinout 74.

Y27.69 plin$ plinout 76.

Y32.69 plin$ plinout 78.

G00 Z73.991 prapid$ prapidout 80.Rapid out OK

X-394.455 Y-45.5 prapid$ prapidout 82.Reposition to next multi pass OK

G01 Y-23.5 Z33.841 plin$ plinout 132.Bad line of code??? Z on sepperate line needed??

Y27.69 plin$ plinout 134.

Y32.69 plin$ plinout 136.

G00 Z73.991 prapid$ prapidout 138.Rapid out OK

X-388.455 Y-45.5 prapid$ prapidout 140.Reposition to next multi pass OK

G01 Y-23.5 Z33.841 plin$ plinout 190.Bad line of code??? Z on sepperate line needed??

Y27.69 plin$ plinout 192.

Y32.69 plin$ plinout 194.

G00 Z73.991 prapid$ prapidout 196.

M09 peof$ peof$ 198.

G00 G91 G28 Z0. peof$ peof$ 198.

M05 peof$ peof$ 198.

 

Thanks

[?Mark]

David.

Does it happen on retract only?

[DavidB]

It happens after the first pass the tool Rapid retracts in Z Rapids to next pass start position then Feed moves in Z- and also the direction of lead in cut.

 

code:

---

 T8 M6

G00 G54 G90 X-422.455 Y-45.5 A90. B90. S640 M03

M12

M10

G43 H8 Z73.991

M08

Z33.841

G01 Y-23.5 F230.

Y27.69

Y32.69

G00 Z73.991

X-394.455 Y-45.5

G01 Y-23.5 Z33.841-- Z should be previous line

Y27.69

Y32.69

G00 Z73.991

X-388.455 Y-45.5

G01 Y-23.5 Z33.841-- Z should be previous line

Y27.69

Y32.69

G00 Z73.991

M09

G00 G91 G28 Z0.

---

[?Mark]

Shot in the dark but try turning retract off in the ops, use cleaRance only and see what happens...

[Tim Johnson]

I'm guessing you have the clearance on in the first op and not on in the second.

 

Edit: on second look I'm thinking Mark's right. Someone else should guess so I can say they're right.

[DavidB]

Mark,

I tried Clearance only with No retract same G-gode.

I tried both retract and clearance some thing.

[?Mark]

Sorry, can't help you here. Maybe Tim has better idea...

[Midwest]

Does it look right when you backplot in Mastercam???

[Tim Johnson]

Is there a chance your construction/tool planes are not the same?

[DavidB]

Planes are correct,backplot is good

 

linky

[Tim Johnson]

What if you set your feed plane inc. 0.5 and plunged at maximum feedrate. Just throwing out ideas.

[Midwest]

quote:

---

multi pass 2d contour toolpath

---

Why are you getting so many Y moves????? Is it a spline and not a line?????

 

 

quote:

---

Z33.841

G01 Y-23.5 F230.

Y27.69

Y32.69

G00 Z73.991

---

A Spline causing problems?????

[Midwest]

quote:

---

How can I get the tool to rapid to the next depth of cut instead of feeding from Top of stock?

---

Inc. has always worked for me.

 

 

Can you post a screen shot so I can see you settings ????

 

 

I left my hasp at work.....

[Midwest]

Try turning cutter comp on...........don't know if you can use it this way, just wondering if it fixes the yz issue.

 

[DavidB]

Mid,

The contour lies in the Y axis the first Y move is the lead in move where the tool rapids too. The next Y the start of the contour the 3rd Y the end point of the contour and the final Y move is the Lead out move.

 

 

I have tried with Clearance also and Clearance only.

This is posted code of above toolpath...

code:

---

 G91 G28 Z0.

( 40MM TIPPED TOOL TOOL - 8 DIA. OFF. - 28 LEN. - 8 DIA. - 40. )

( FACE BACK OF PART )

M13

M11

T8 M6

G00 G54 G90 X-422.455 Y-45.5 A90. B90. S640 M03

M12

M10

G43 H8 Z73.991

M08

Z33.841

G01 Y-23.5 F230.

Y27.69

Y32.69

G00 Z73.991

X-394.455 Y-45.5

G01 Y-23.5 Z33.841??????

Y27.69

Y32.69

G00 Z73.991

X-388.455 Y-45.5

G01 Y-23.5 Z33.841???????

Y27.69

Y32.69

G00 Z73.991

M09

G00 G91 G28 Z0.

---

[Colin Gilchrist]

David,

 

In your control definition look at the "Linear" page. Enable the radio button under XY plane control to "Break rapid moves - XY then Z for approach, Z then XY for retract". That should put all Z motion on seperate lines. If it does not, then your post might not be set up to take advantage of this feature. I know the MPMaster post supports this. So do all of the new "generic" posts that shipped with X.

 

FYI, you should be able to get an install disc from your reseller with something like 26 generic Mastercam posts for X. There is a Fadal, Haas, Mazak, Mori-Seki, Okuma, and a few others.

 

HTH,

 

Colin Gilchrist

The Boeing Company

MR2 and Beta test site

[Colin Gilchrist]

Hi David,

 

Look for the "nobrk$" setting in your post general output settings. This should be set to "no$".

[DavidB]

Hi Colin,

From my control def...

 

From my post

code:

---

 nobrk$       : no$    #Omit breakup of x, y & z rapid moves, option 2 is not valid

#Option 2 not valid, only with table/table types

---

[Colin Gilchrist]

Hmmm... Then I would check the prapid and plin post blocks for the Z output...

 

[DavidB]

code:

---

 prapidout       #Output to NC of linear movement - rapid               

pcan1, pbld, n$, `sgcode, sgplane, sgabsinc, pccdia,

xout, yout, zout, p_out, s_out, strctxt, scoolant, e$

 

plinout #Output to NC of linear movement - feed

punclamp

pcan1, pbld, n$, `sgcode, sgplane, sgabsinc, `sgfeed, pccdia,

xout, yout, zout, p_out, s_out, `feed, strctxt, scoolant, e$

if nc_lout$ <> m_one & feed = zero, psfeederror

pclamp

---

code:

---

 plin0$           #Linear movement, set brklinestype        

---

[Tim Johnson]

Try changing your top of stock to inc .5 and see what happens.

[Midwest]

Shutoff lead in/out

 

 

Don't see why you need this if you aren't arcing in and out with cutter comp.........you are just staying in a vertical path.

[DavidB]

The line is tacken from a solid edge so a lead in of 55% cutter diameter is needed also a lead out is needed.

[Tom Dorgan from American Precision]

How about if you check keep tool down in the multipass options dialog box?

[DavidB]

Keep tool down is not an option in this case.

I'm sure my problem is post related not what I've done in MC itself?