Mplmaster Update

[Post dept]

All,

 

Little update to mplmaster and a couple of added features.

 

1. New switch called g54g55 to force G54 for all main spindle ops and G55 for all sub spindle ops. No need to set your work offset anymore.

 

2. Misc int 10 for turning ops - "CRF X value [0=orig,1=post]". This fixes the problem where you have a rapid from the end of your canned rough to the beginning of your canned finish and it goes through the part after the finishing canned cycle. The only programming limitation is that your canned finish must follow the canned roughing routine whose pattern it uses. It does not have to be right after, but must be before any other canned ops. Search for #CRF to implement this in your existing posts.

 

3. Forced output of the proper ijk values for milling. This was never really working properly in any of the lathe posts but I believe it is now.

 

Brett

[Wise-ACR]

Is this available now?

[Post dept]

Yes, it's up on the mplmaster page.

[Post dept]

I should also send a big thanks to MillingMan for his help on this. He was instrumental in getting the misc int 10 functionality added.

[crazy^millman]

Brett,

Could you guys update the web site the date does not reflect this and could confuse a lot of people.

 

Oh yeah Brett thanks I just got done with my Okuma post now I need to changes this new to match.

[Post dept]

Yup, date needs to be changed. Thanks.

 

I waited until you got your Okuma post done to put this up.....can't make things too easy for you.

[crazy^millman]

Haahahah Yeah well you guys make it a lot easier than CNC does so I take my lumps where I must.

[Mick]

I cant thank Inhouse enough. These guys are great, and an asset to Mastercam users worldwide.

[kenfromlodi]

Any plans on fixing the G73 Pattern Repeat Cycle?

Never worked right?

[Dan@home]

Brett & MillingMan.

[Randy Morton @ Clem Industrial]

*blush*

 

Ken, what wrong with the G73? I use it quite frequently and don't recall ever having issues with it. I did have to tweak my post so the initial retract was a non-decimal number (for X & Z), but other then a 'machine specific' thing, works great for me. Can you post up some code?

[Post dept]

I see you've switched from MillingMan to Randy @ SFI.

 

Thanks for your help on it.

[kenfromlodi]

I can and I would love to get it straightened out.

I have sent a zip2go to a couple very good guys on this site and they were unable to find the problem either. I do not get any I or K values on a OD cycle and the if its an ID cycle it will take the largest diameter and put the I at just about half and Im not sure where it gets the K value. (putting the I at half is fine for small parts but does not work well on large parts because the number is way to big) heres some code::

 

( ROUGH TURN OD )

X15.1565

Z.0885

G73 P100 Q110 I0. K0. U.01 W.005 D5 F.01

N100 G0 X9.75 S350

G1 Z-.0032

G3 X10. Z-.1563 I-.0313 K-.1531

G1 Z-2.4063

G2 X11.9375 Z-3.375 I.9688

G1 X12.9375

G3 X15. Z-4.4063 K-1.0313

N110 G1 Z-6.02

G0 Z.0512

 

 

(ROUGH BORE)

G0 X5.9114 Z.0963 M8

G73 P120 Q130 I2.9557 K.0963 U-.01 W.005 D5 F.01

N120 G0 X8.25 S350

G1 Z-.0032

G2 X8. Z-.1563 I.0313 K-.1531

G1 Z-3.7813

G3 X7.5625 Z-4. I-.2188

N130 G1 X6.06

G0 Z.0512

 

 

Thanks for any help.

[Post dept]

kenfromlodi,

 

E-mail me your zip2go.

 

Brett

[kenfromlodi]

Brett,

 

I sent it over, thanks for taking a look.

[chowquoe^]

Brett,

 

Any of these changes affect the Integrex post?

[Post dept]

Not sure.....its a Mits control so I'm not sure how people are doing with the canned rough and finish thing. I did change the forced arc ijk but if you're not having problems...no worries. g54g55 does not apply.

 

Brett

[Rakesh]

Brett,

Mplmaster from the post site, when I download,only have lmd,control and pst file and don't have the mmd file. Is this missing or to be created by ourself?

thanks

[Rakesh]

Sorry Brett, It should be lmd file instead of mmd.

[Post dept]

All,

 

I have found the problem with the G73 pattern repeat.

 

To recap, his problem was to do with the UW vector for pattern repeat G73 not coming up with the right values.

 

code:

---

 

pl_ncoutput #Movement output

pcc_capture #Capture LCC ends, stop output RLCC # 05/28/04 #This was previously commented out but I have removed that as it affects G73 pattern repeat. I'm not sure what else this affects at this point. WBT

 

---

I hope this helps anyone that uses G73....and I hope it doesn't break anything else! I'll send it into CNC for them to take a look at.

 

Brett

[Randy Morton @ Clem Industrial]

Maybe that is why mine worked? Mine was not commented out...strange since all my current posts are based off the MPLMaster prior to the revision of the G70 fix as per above...weird.

[Post dept]

Huh....no clue on that one. Mplmaster didn't exist in 2004 so this is an mpfan thing.

[Post dept]

All,

 

Further info on that G73 item as discussed above.

 

Uncommenting the call to pcc_capture is step 1. However, this will blow away the z motion after the canned cycle due to the setting of the no_nc_out$ flag. To fix, go to pcc_capture and make the following change.

 

code:

---

 pcc_capture     #Capture ends of canned turning path, stop output w/rough

#Stop output in rough only lathe canned cycles

#between rough and finish paths

#if cc_stop_fcc & rcc_flg$ = 6, no_nc_out$ = one # 05/28/04

if cc_stop_fcc & rcc_flg$ = 6 & lathecc <> 2, no_nc_out$ = one #wbt - do not want to stop output before/after pattern repeat

---

I hope this helps.

 

Brett

[Kyle Waters]

Does anyone else use the live tooling with the spindle? Not sure of other brands, but in our NL, it's an M90/M290. Just curious, I use alot for drilling where I can't make the required RPM with just one spindle.