Number of decimal places for rotary output

[Justin Beebe at Folsom Tool]

I'm trying to run my first part on our new Haas UMC-750 but the machine is giving me an alarm when the B-axis goes to rotate. I believe it is because my post is posting the B move with four places after the decimal point. Three places after the decimal point seems to work. The alarm is alarm number 386 Invalid address format. I tried looking in the machine definition, control definition, and post so I can change the setting to post three decimal places only but can't find it. Can someone show me how to do this. Here is the G-code that is causing the alarm.

 

 

O1971

 

(MCX FILE - C:\USERS\JUSTIN.BEEBE\DOCUMENTS\MY MCAMX6\MCX\CUSTOMERS\BOEING\901-031-523-157\901-031-523-157-JB.MCX-6)

 

(T3 - 3.00 FACEMILL WITH .125 RADIUS - H3 - D3 - DIA 3." - CORNER RAD .125)

 

N100 G00 G90 G17 G20 G40 G80

 

N110 G53 Z0.

 

N120 G53 X-30. Y0.

 

(FACE TOP)

 

N130 T3 M06

 

N140 G00 G17 G90 G54

 

N150 S6000 M03

 

N160 M11 (C-AXIS UNLOCK)

 

N170 M13 (B-AXIS UNLOCK)

 

N180 B5.5418 C-90. --------------------------- This B move with four decimal places is the problem

 

N190 M10 (C-AXIS LOCK)

 

N200 M12 (B-AXIS LOCK)

 

 

Thanks in advance,

 

Justin

[crazy^millman]

Is this the dialed in post from CNC Software's post department? If so shoot off an email to them and see what they can do to help you dial it in. There should be a formant statement somewhere tied to that axis output. Should be a simple change, but without having everything in front of mt to review would be hard to know exactly where and what needs to be adjusted.

[Justin Beebe at Folsom Tool]

Crazy thanks for the suggestion. I fixed the problem by making the following changes to the post. You can see the changes on the lines I initialed with #JB

 

 

 

 

# Coordinate Formats

 

# --------------------------------------------------------------------------

 

fmt "X" 2 xabs

 

fmt "Y" 2 yabs

 

fmt "Z" 2 zabs

 

fmt "X" 2 xabs_top

 

fmt "Y" 2 yabs_top

 

fmt "Z" 2 zabs_top

 

fmt "X" 3 xinc

 

fmt "Y" 3 yinc

 

fmt "Z" 3 zinc

 

fmt "X" 2 xhome

 

fmt "Y" 2 yhome

 

fmt "Z" 2 zhome

 

fmt 11 rotabs # JB WAS 2 CHANGED TO 11 FOR 3 DECIMAL

 

fmt 11 tiltabs # JB WAS 2 CHANGED TO 11 FOR 3 DECIMAL

 

fmt 3 rotinc

 

fmt 3 tiltinc

 

fmt 3 rotdelta

 

fmt 3 tiltdelta

 

I'm not sure if I need to make the same changes on the rotinc and tiltinc lines.

 

Also this post is having another issue.

 

If I post a toolpath in the top tool plane all of my Z values are correct. When I post with other tool planes the Z values are not correct. For example when B is rotated 5 degrees and I have my clearance plane set to absolute 10.500 inches in mastercam the post will post out 10.509. If I post in the front plane and I have Z set to absolute 2.000 inches in mastercam the post will post out Z 4.000 inches. I'm sure I have my mastercam file set up properly so it must be something with the machnine def, control def, or Post. As a test I posted the same file with a machine def and post that we have been using for a few years and it gives me the correct z numbers. I'm going to call our reseller tomorrow and try to get everything straightened out.

[Masterminder408]

Yeah, I had the same problem with the B-axis posted out 4x place,,, thanks i'll try to change that in the post....

 

one question, how come you didn't out put " G254" which is DWO, on your post?, I used mine with no problem, everything is TOP/TOP in WCS..., you do not have to use different plane.... DWO and TCPC knows exactly where you at....and did you check the WIR? self center that will out put to parameter # 106 for X, #107 for Y, both Xand Y Center of B axis, and #108 is for Z which is center of C axis...., then put those in #1306, #1307, #1308, manually,...

 

The post work great...DWO and TCPC worked great, tested a couple part with no problems...

 

The only problem is X/Y/Z axis, everything is over hang so much, that I'm afraid to put everything at 100% rapid... Haas gotta redesigned there machine structure.... the rotary seem to be ok... plus the original plate is one of the most irritated ....

 

We 're going to take the sub plate Haas' creation of " watchout, you 're going to need a lot of clearance, sub plate ever" and create a disk, similar with TR210...

[Justin Beebe at Folsom Tool]

Crazy,

 

I forgot to mention that this is the Post from In House that is supposed to be dialed in. We have purchased many posts from In House in the past and we are always pleased with them. Most of them do require a few tweaks once you get them and start using them. When something needs to be tweaked that is above the scope of my knowledge we usually send the post to our reseller then they get in touch with In House and once In House makes the changes the reseller sends it back to us. I'm going to send it to our reseller tomorrow.

 

Mastermnind408,

 

I turned off the switches in the post for DWO and TCPC because we are programming from the center of rotation and machining from solid blocks of material with no previous machining operations done to them. The parts are located on the machine in the same place they are programmed from in mastercam and we machine them complete in one operation. We had a technichian from Haas come out and set up the machine. He ran the probe and entered all the numbers in the parameters for the Machine Rotary Zero Point. Since we are programming from the center of rotation we copied those numbers into the G54 work offset and now we can program parts from the center of rotation without ever having to probe anything or pick up a part zero. Like I say now the problem I'm having is the post isn't posting out the correct numbers that I have set in Mastercam when I use any tool plane other than top. On a side note I hear what your saying about the clearance issues with the platter. I designed a fixture that gets the parts up off the table. Once I get this post problem fixed I'm going to start making some parts then make adjustments to the fixture if needed. I'm glad to know you have the same machine. Let me know if I can be of any assistance in the future. We may both encounter some of the same issues.

[Masterminder408]

Justin,

Yeah, don't worry we 'll keep in touch , since I haven't done any "full 5" yet, just 3+2 until I'm confident with it..

I got what you were saying about taking DWO and TCPC off....to me it is to our "programmers" advantage to use it.... it make programming in mastercam so much easier... I understand that you machine from a solid block and there is no need for DWO and TCPC... I 've tried "2nd Op" with probe, DWO, and it worked flawless, I have use with "1st Op" with probe, rotated in 3+2 mode and it worked flaw less... the point here is I don't have to move the part in mastercam, just TOP/TOP and forget about moving the part else where to match the center rotation of C and B axis... reason is that when I used my VF3-TR210, everytime new set up "repeat job" the center point is off,,, so I did it this way, for every top/top I used separated work offset which base on top of part, for every angle I used a macro to calculated from known centerpoint and added in different work offset... this is the only way for me not to mess with moving the part ever again.... UMC 750 has that feature, I'm so glad that it did....

and again, yes Haas 's plate is definitely a minus ... till this day I can't think of the reason why they have to make their plate rectangle instead of a round smaller plate... but don't worry I'm gonna take it off and make a round plate, if you have the machine 's skeleton you 'll see there are only 6x screws to hold it together with table...

 

regarding your original problem, it did not happened to me,,, the post work flawlessly

probably something is not right with your MMD/CMD or PSB files...

 

Nguyen.... keep intouch, I 'll keep you update on everything about UMC-750...

[Justin Beebe at Folsom Tool]

Thanks, Mastermind408 I will do the same.

[Masterminder408]

Justin,

 

You 're right, if you have the DWO and TCPC switch to "0"in the post, then you have issue with the Z depth... i'll send it in to QC...