captaingamez Posted November 12, 2014 Report Share Posted November 12, 2014 I had to recently setup a machine that was not setup from origin point, but ran a 4th axis, multiple offset setup. In this setup there is an offset for each angle and plane which is machined on. There were 6 offsets for op1 and 2. Six......., versus having them all done with 1 that the positions NEVER change, and can be used on every part programmed this way in this machine. Quote Link to comment
Mattndew76 Posted November 12, 2014 Report Share Posted November 12, 2014 I had to recently setup a machine that was not setup from origin point, but ran a 4th axis, multiple offset setup. In this setup there is an offset for each angle and plane which is machined on. There were 6 offsets for op1 and 2. Six......., versus having them all done with 1 that the positions NEVER change, and can be used on every part programmed this way in this machine. I have dealt with those type of programmers before. Manufacturing has no need for them. Worked with a lathe programmer once that thought it was cool to put an offset on every surface turned. Quote Link to comment
captaingamez Posted November 12, 2014 Report Share Posted November 12, 2014 I have dealt with those type of programmers before. Manufacturing has no need for them. Worked with a lathe programmer once that thought it was cool to put an offset on every surface turned. I have heard of that too, Thats an awesome way to destroy a lathe. we always use the exact same point for programming in the lathe. Quote Link to comment
Mattndew76 Posted November 12, 2014 Report Share Posted November 12, 2014 I trashed the idiots programs and rewrote them every time they hit the floor. He didn't last very long as an employee. Over sold himself and got exposed for the fraud he was. Quote Link to comment
q-tip Posted November 12, 2014 Report Share Posted November 12, 2014 I trashed the idiots programs and rewrote them every time they hit the floor. He didn't last very long as an employee. Over sold himself and got exposed for the fraud he was. We get a lot of guys like that, but they tend to hang around a while... Quote Link to comment
Mattndew76 Posted November 12, 2014 Report Share Posted November 12, 2014 We get a lot of guys like that, but they tend to hang around a while... I know your situation. Are they now managers? 1 Quote Link to comment
q-tip Posted November 12, 2014 Report Share Posted November 12, 2014 :rofl: you know exactly how it is :lol: 2 Quote Link to comment
mklotz70 Posted November 12, 2014 Author Report Share Posted November 12, 2014 I've got the second "s" in "kiss" down pat!!! :) Very interesting information guys! Thanks!!! It may be some time before I even pull out my 4th axis, but I'm still trying to learn what I can for when the time comes. I've been working on my new mill a little each day....it's down to some tweaking now. :) Quote Link to comment
Josh K. Posted November 12, 2014 Report Share Posted November 12, 2014 On our Horizontals we program to corner of part/stock and have MasterCam output G10 lines to shift the origin. I hate centerline on HMC's.... On VMC's with rotaries (which I haven't done in a few years) I do the same. I like having my z values relative to the part and not centerline. Sometimes I program from center of rotary. It really depends on the part. If it's a 4 sided fixture/tombstone I'll program from faces. If it's a single part I'll go centerline. Multiaxis lathes its always G54 for main, G55 for sub. Centerline of course. 5axis Mills it's always center of rotaries. We use G10 lines to write most all of our work offsets using subplates and charts to tell you the exact location. Takes 30sec to load your work offset. No edge finders... HMC's its just load gcode and hit cycle start. Quote Link to comment
Josh K. Posted November 12, 2014 Report Share Posted November 12, 2014 If your doing high precision work you need lots of offsets. I have a family of parts running on a HMC and the parts have as much as 12 offsets each. Each rotation has to be adjusted independently. You guys are talking about two different methods. Center of rotary. Shifted work offset. I use both where applicable. Some guys are either one or the other. Old school (centerline) or new school (shifted). Josh- Quote Link to comment
dr.feltersnatch Posted November 12, 2014 Report Share Posted November 12, 2014 I prefer centerline. And since I run up to 24 jobs at a time g10's are a must. Why dont you like centerline josh? Quote Link to comment
Josh K. Posted November 12, 2014 Report Share Posted November 12, 2014 I like my depths and retracts relative to the part. When I see Z.25 it makes sense. When I tap a part and see Z-.535 it makes sense. My post outputs all the g10 lines for me. I'll post sample code when I get to work. 1 Quote Link to comment
Josh K. Posted November 12, 2014 Report Share Posted November 12, 2014 Here's a typical HMC code output: % O0123(14-0779) (POST REV 2.0) (NH4000DCG - HMC) (MCX FILE - 421Z6301-4062--B-CELL.MCX-8) (DATE - APR-29-2014) (TIME - 5:09 PM) (USER ID - ***) (OPERATIONS - 50/60/70) #510=21(OPTIONAL N SEQ START) IF[#510EQ1]GOTO3000 M0 (USING OPTIONAL N SEQ START) M0 (YOU ARE STARTING PART WAY THROUGH) N3000 (*** TOOL LIST ***) (T1 - I321 -3" FACE MILL - D3.0000 - R0.0313) (T6 - B682 - 0.250" END MILL - 0.01" RAD - D0.2500 - R0.0100) (T12 - O600 - 1/4"-90 SPOT DRILL - D0.2500) (T31 - D1236 - #16 DRILL - D0.1770) (T15 - F1829 - 0.1985" REAMER - D0.1985) (T8 - B3470 - 1/2" END MILL - 0.094" RAD - D0.5000 - R0.0940) (T4 - B3533 - 3/4" ENDMILL - D0.7500 - R0.0300) (T27 - D2354 - 5/8" DRILL - D0.6250) (T28 - B3460 - 1/2" END MILL - D0.5000 - R0.0200) (T5 - B3461 - 1/2" ENDMILL - D0.5000 - R0.0300) (T13 - D1727 - 0.386" DRILL - D0.3860) (T9 - B3473 - 3/4" ENDMILL - 0.094" RAD - D0.7500 - R0.0940) (T16 - B572 - 1/2" END MILL - 0.008"RAD - D0.5000 - R0.0080) (T29 - B1357 - 1/2" END MILL - 0.0625"RAD - D0.5000 - R0.0625) (T25 - B2956 - 3/8"BALLNOSE - D0.3750 - R0.1875) (T30 - B1367 -3/16" BALLNOSE - D0.1875 - R0.0938) (T26 - L352 - 0.250"X45 CHAMFER MILL - D0.2500) (T18 - TD3475 - ROMICRON BORING HEAD - D1.0003) (T19 - TD3095 - ROMICRON BORING HEAD - D0.7500) (T20 - J2537 - 0.500"X45/-45 BACK CHAMFER - D0.5000) (T22 - A2432 - 0.1875" END MILL - D0.1875) (T23 - F3476 - 0.2545" REAMER - D0.2545) (T24 - F567 - 0.3135" REAMER - D0.3135) (*** USER DEFINED WORK COORDINATES START ***) (TOOL PLANE - OP60 - B0 - P1) G90G10L20P1X0.Y6.9061Z10.2425B0.(ACTUAL - B0. FACE) G91G10L20P1X0.Y0.Z0.(INCREMENTAL WORK SHIFT) (TOOL PLANE - OP60 - B270 - P2) G90G10L20P2X10.2425Y6.9061Z0.B0.(ACTUAL - B270. FACE) G91G10L20P2X0.Y0.Z0.(INCREMENTAL WORK SHIFT) (TOOL PLANE - OP60 - B90 - P3) G90G10L20P3X-10.2425Y6.9061Z0.B0.(ACTUAL - B90. FACE) G91G10L20P3X0.Y0.Z0.(INCREMENTAL WORK SHIFT) (TOOL PLANE - OP60 - B0 - P4 - SLOT FINISH) G90G10L20P4X0.Y6.9061Z10.2425B0.(ACTUAL - B0. FACE) G91G10L20P4X.002Y0.Z0.(INCREMENTAL WORK SHIFT) (TOOL PLANE - OP60 - B0 - P5 CENTER FEATURES) G90G10L20P5X.0012Y6.9061Z10.2425B0.(ACTUAL - B0. FACE) G91G10L20P5X.001Y0.Z0.(INCREMENTAL WORK SHIFT) (TOOL PLANE - OP70 - B0 - P25) G90G10L20P25X-1.9647Y13.438Z7.4385B0.(ACTUAL - B0. FACE) G91G10L20P25X0.Y0.Z-.0006(INCREMENTAL WORK SHIFT) (TOOL PLANE - OP70 - B355 - P26) G90G10L20P26X-1.3089Y13.438Z7.582B0.(ACTUAL - B355. FACE) G91G10L20P26X0.Y0.Z0.(INCREMENTAL WORK SHIFT) (TOOL PLANE - OP70-B221.795-P27) G90G10L20P27X-3.4958Y12.7695Z6.8468B0.(ACTUAL - B41.79 FACE) G91G10L20P27X0.Y0.Z0.(INCREMENTAL WORK SHIFT) (*** WORK COORDINATES END ***) GOTO#510(JUMP TO SEQ) M01 N1(Sequence #1.) (TOOL# 1 - I321 -3" FACE MILL - DIA. - 3.) (OP 22 ) (MAX - Z.02) ( PALLET CHECK - PALLET2 ) M500C2 G00G17G40G80G90G53Z0. T1M6 M11(UNLOCK) G00G17G90G54.1P25B0. M10(LOCK) X-2.3186Y2.5659S6000M03 G43H1Z2.M8T6 G332R1. G5P10000 Z.25 G94G01Z.14F100. P1-24 are assigned to Pallet 1, 25-50 are assigned to Pallet 2. The post outputs the correct pallet change number per work offset. ( PALLET CHECK - PALLET2 ) M500C2 In this case it's pallet 2. You'll also notice the following: (MAX - Z.02) Since the work offset is set to "Top of finished part", this will tell you exactly how deep that tool will go. In this case it will Leave 0.020" on the part face. Very handy for validation at the control. -Josh Quote Link to comment
Mattndew76 Posted November 12, 2014 Report Share Posted November 12, 2014 If & GoTo loops. Used those a ton on the Okuma Pallet change horizontal. Each face of the tomb stones had its own quardinate call out, and P-# Loved how I could set the tools from the tool setter and park them in the belt. A probe would verify rough stock and finish part dimension as well. Lights out. Quote Link to comment
Josh K. Posted November 12, 2014 Report Share Posted November 12, 2014 Probes are great. As long as their not old Renishaw continuity probes.... The sequence start (#510, coincidence?) is setup so if you need to start part way through you are A) Informed/warned that is what you're doing. B.) So the work offsets are written and updated incase you made a change since last time they were written. Quote Link to comment
Mattndew76 Posted December 5, 2014 Report Share Posted December 5, 2014 I just gotta come out and say. Volume milling is the shit!! Quote Link to comment
Josh K. Posted December 9, 2014 Report Share Posted December 9, 2014 High speed machining is the way to go. Here's part #2 of 4 different parts 3 Quote Link to comment
Uber Deaf One Posted February 2, 2015 Report Share Posted February 2, 2015 Thread revival! Couldn't find the machining pr0n thread so this will have to do...One of our two new 5 axis machines came in.. w00t! 4 Quote Link to comment
Mattndew76 Posted February 2, 2015 Report Share Posted February 2, 2015 Wish I had the backorders to support buying one of those!! Quote Link to comment
dr.feltersnatch Posted February 2, 2015 Report Share Posted February 2, 2015 I always liked matsuura. Quote Link to comment
q-tip Posted February 3, 2015 Report Share Posted February 3, 2015 You guys get the fancy machines and I'm machining a beryllium casting with a machine from the stone age. But I get to use carbide tools so I have that going for me. 1 Quote Link to comment
Mattndew76 Posted February 3, 2015 Report Share Posted February 3, 2015 Lol. That's how I feel running this HAAS VF4 at work. Talk about a heap of turds. But I can use carbide lol Quote Link to comment
captaingamez Posted February 3, 2015 Report Share Posted February 3, 2015 Nothing wrong with a good ol VF4. Some of us have to be happy with what we get. And we have make incredible results with that. That Matsuura is sexy though. Quote Link to comment
Mattndew76 Posted February 3, 2015 Report Share Posted February 3, 2015 Nothing is wrong with VF4. Maybe you misunderstood me. I mean this specific pile of turds at this company. 1 Quote Link to comment
Recommended Posts
Join the conversation
You can post now and register later. If you have an account, sign in now to post with your account.
Note: Your post will require moderator approval before it will be visible.