Posting error

[Kenneth Potter]

Ok

I have a single surface "Human nose" to machine that has undercut areas . I'm using a lollipop. I rotated the cplane at a a slight angle & set the tool plane to top. That allows the lollipop to perform the undercut. When i post it with mpfan.pst i get a error message"

Seletor varitable plane=1.0

out range for string select. ??????

At this point posting is interupted at the tool that has the rotated plane.

 

 

Can someone tell me what does this means & how i can fix this.

Mill V8 mpfan.pst cd

Kenny

[This message has been edited by Kenneth Potter (edited 12-27-2000).]

[Greg McKay]

I have forwarded your question to R. taft in the post department

[Kenneth Potter]

Thanks Greg for the forwarding But long distance from,my end is a no no.My work around for now is a using post that out puts only X,Y,Z& no TM6 ,dia,H table or spindal speed. post one tool a time with a lot of editing

till i figure this out.

Thanks Anyway

Kenny

[This message has been edited by Kenneth Potter (edited 12-27-2000).]

[Rich Taft from CNC Software]

Ken, The error message you received is indicative of an NCI problem, but you can work around it in the post by validating the plane variable prior to accessing the string select function. The less desirable alternative would be hand editing the ASCII NCI prior to posting, or using the runold C-hook to force the variable to zero (Version 6 and earlier Mill posts), but you will lose too much information to make that a feasible workaround.

If you decide to work around it in the Post Processor (I thought you might) you should be able to get away with adding the following line of code to the ‘pcom_moveb’ postblock of MPFAN (indent at least one space).

if plane < zero | plane > two, plane = zero

This should do the trick.

Best Regards,

Richard Taft

Post Processing Services

CNC Software, Inc.

671 Old Post Road

Tolland, CT USA http://www.mastercam.com

 

[Kenneth Potter]

i made the changes & still have the same error

this is how i added the new line

 

pcom_moveb

if plane < zero | plane > two, plane = zero

c_mmlt #Multiple tool subprogram call

ptoolcomment

comment

pcan

if stagetool >= zero, pbld, n, *t, "M6", e

pindex

if mi1 > one, absinc = zero

pcan1, pbld, n, *sgcode, *sgabsinc, pwcs, pfxout, pfyout,

pfcout, *speed, *spindle, pgear, strcantext, e

pbld, n, "G43", *tlngno, pfzout, scoolant, next_tool, e

absinc = sav_absinc

pcom_movea

toolchng = zero

c_msng #Single tool subprogram call

[Rich Taft from CNC Software]

Ken,

You should add the code snippet to the ‘pcom_moveb’ postblock. A postblock definition always starts in the first column. The indented ‘pcom_moveb’ you found is actually a “Call” to that postblock. Try searching for the postblock again and just hit “find next” until you see the word ‘pcom_moveb’ in the far left column. When you find it open up a line below and insert the code (don’t forget about the indentation).

If it still gives you trouble, you can just email me and I’ll send you an edited post and you can compare the two.

Best Regards,

Richard Taft

Post Processing Services

CNC Software, Inc.

671 Old Post Road

Tolland, CT USA http://www.mastercam.com

 

[Webby]

When listing postblocks on this forum it is helpful to use the UBB Code tag along with an HTML BIG code. Without it, your idents and spacing will be lost. Click on Edit for this message to see how it's done:

code:

---

plinout         #Comment
      this area maintains formatting

---

[This message has been edited by Webmaster (edited 12-29-2000).]