Work offsets Mill

[AETOOLS]

I seem to be having a problem. This is the first time I have had to program in mill for a production job. My problem is I have 4 work pc's I just want my program to change my G54 to G55 G56 etc. I did the transform toolpath thing but have found I can only get it to do 2 work offsets G54 and G55. No matter what I do it will only create 2 parts not 4 5 or 6. The other thing I can't get it to do is run all parts with first tool then goto next tool. It wants to run all the tools on first part then run all the tools on second part. I am in a crunch here.

thanks

 

Joe

[Guest]

OK well the order of the tools can be taken care of by changing your Group NCI output by, change it to "operation order"

 

To try added offsets, try clicking on Tool Plane >> Work Offset numbering, click assign new >> start 0, increment 1. On the translate tab >> Click rectangluar >> X and y spacing set to zero, X steps 4 y steps zero

 

Try that and see what you get.

 

It should give you 4 spacings and G54, G55, G56, G57.

[AETOOLS]

I have to start 1, incement of 1. If I do 0 and 1 it starts with G55 then goes to G54. Have all the rest with the same settings as above, but still only get 2 work offsets, (G54,G55) and it runs threw all of the operations in G54 then does them all again with G55. So you can see my problem!!!

[AETOOLS]

Also will not output program number. Only outputs O0

[Guest]

You got this post by running your V9 thru the update utility?

 

If so, there should be a log file for your post, you might want to read it and see if everything updated cleanly.

 

Also, what are you using for a post? mpfan? mpmaster?

 

Have you tried right clicking >> edit slected operations >> change program number.

 

Then regen and see if you get a #

[AETOOLS]

Yes V9 updated to X post name it MPHAAS_NO-AX.PST I was able to get the progam number to come up, but nothing else has changed. I have tries other post's that came with X and a file my vendor send me but all only post 2 work offsets and they run all tools 1 part instead of 1 tool all parts

[Guest]

Why don't you down load the mpmaster from this site and try that just for sh*ts and grins.

 

If that still behaves the same way I'd be glad to take a look at it for you.

[AETOOLS]

Where do I find mpmaster? I just did an update on mpfan and no change.

[AETOOLS]

Ok did the mpmaster thing. Tried it twice. gets about 1/3 of the way posting and locks up my machine. When can I star typing in all upper case letters. This is really starting to P me off. I am only trying to do something simple. I know I still have a lot to learn with Master Cam, but I am the one that made the decision to switch to Master Cam from out other program. This is a simple thing to do in our other program but then that one lacked a lot or I would not have wanted to switch. HELP (didn't reall mean to type that in all upper case)

[Guest]

check your mail

[g huns]

When I try to transform to differnt fixtures I get the ops grouped how I like but no differnent work offset #'s. First op is at G54, it copies that op but just runs again at G54. I have assign new checked for work offset numbering, start-1 increment 1. Doesn't seem to matter what #'s I put in the blanks either, except 0. I'm thinking I new to tweak something in my post but have no clue what.

[Guest]

I don't know if this will help you I usually do it as start 0 and increment of 1

 

What does a 0 get you for output?

[g huns]

O still gets me G54, unless I turn off "set to post values when posting" on the misc values page. Then I get nothin for work offset.

[Guest]

What post are you using?

[g huns]

#| MASTERCAM MP POST PROCESSOR | Always back up your post-processor |

#| CNC Software, Inc. | prior to making any changes. It's easy, |

#| Control Model: YASNAC MX3 | just put a floppy in drive a:, at DOS |

#| Machine Model: GENERIC | type "COPY C:MILL55*.PST A:" |

#| PST File Name: YASNAC.PST/TXT | |

#| Executable : MP.EXE 3.12

 

That's the one our reseller gave us when we got MC. Never had the balls or time to make my own. Never been jumpin up and down happy with it but it works 99% of the time.

[Wally J]

There is another post avail in the same location as the MPmaster.. it is the Mpsubrep you can try that but you still have to set the switches inside the Post for your control,, Ex Break arcs,

stage tools, IJK or R , and location of your posted NC files....

 

I will check back to see if you are having any luck..

 

Wally

[DavidB]

This is an interesting topic.

 

quote:

---

To try added offsets, try clicking on Tool Plane >> Work Offset numbering, click assign new >> start 0, increment 1. On the translate tab >> Click rectangluar >> X and y spacing set to zero, X steps 4 y steps zero

---

I did a drilling toolpath at X0 Y0

Transformed as per above,what happened was I got 8 positions.I then transformed in one direction only X 4 times.Got the 4 new toolpaths.Assigned Tplane workoff sets to Increamental 0 by 1.

 

The posted code does not put in a G55,G56,G57,G58.

Post is...

# Description : IHS MASTER GENERIC MILL G-CODE POST

 

John,

 

quote:

---

OK well the order of the tools can be taken care of by changing your Group NCI output by, change it to "operation order"

---

Where is this setting??

 

Thanks

[Guest]

It is on the bottom left corner of the transform dialog page.

[DavidB]

You can only transform one toolpath at a time correct?

 

What if you could transform a whole group of toolpaths that did the whole component, say 15 toolpaths.

 

Transform the Group of toolpaths 4 times outputting G54-G57, also in tool order not Group order.

 

You could machine 1 part complete. Do it in 3 other positions, and all the first op in all 4 positions then the second op and so on.

[Guest]

No David you can transform as many as you want.

 

Use the CRTL button to add addition tool paths.

If you pick all you paths as the transform you can only the work from G54 across. But you can eother do i tool by tool or operation by operation.

 

Also,

 

You can work back and forth across 4 vises lets say. It's a little more work but it is doable.

 

Transform Tool 1 , work offset start 0 increment 1

Transform tool 2, work offset start 3 increment -1

Transform tool 3, work offset start 0 increment 1

 

and you can work back and forth like that.

[CNCme]

Good day,

Did 4 rectangle with transform, asign new, started

work ofs # at 0, incr. 1, tool plane, and

got g54, 55 ,56 , and 57 ok, using generic vert

3 axis????????

 

milling in VX sp1 ver 3

 

I us this alot....works good for me

 

Tony G

CNCiT Precision Machine - Hudson,NH

X Beta Site

Almost Employed Senior Programmer

N.E Massachusetts - Southern New Hampshire

_________________________________________

End mills and tooling are like The "AMMO"

And coolant and chips are like the enemy

Under your boots as you advance in the

Manufacturing Battle

[CNCme]

Good day,

 

JMP,

That should be a setting

G54,55,56,57 then G57,56,55,54

like reverse work ofsets

 

+1 John

 

Tony G

CNCiT Precision Machine - Hudson,NH

X Beta Site

Almost Employed Senior Programmer

N.E Massachusetts - Southern New Hampshire

_________________________________________

End mills and tooling are like The "AMMO"

And coolant and chips are like the enemy

Under your boots as you advance in the

Manufacturing Battle

[g huns]

It was my post that wasn't making it come out right. I downloaded the new mpmaster and it posts great, even posts out G54 P1, P2, P3..... if you set the starting work coord. at 6, way cool. Now I just need to tweak a little to try and match the way my old post did everthing else. So I'm sure more questions will follow.

[Guest]

Yes, a reverse path switch there would be a nice addition.

[AETOOLS]

Wow, I have been away sinse I started this thread. I was able to get offset working. Was a prob with post and my settings. The one thing I have noticed that stinks is if you have a tool doing more then one operation, regardless of how hard I may try it will run the first op with that tool in each offset then come back to the firt offset run the next op then go back again. Another program I use to use you could choose by operation type or by tool. Was a very nice feature so once it grapped a tool it would do all of the operations that tool needs to do on the first work offset then move to the next.