Probing with G68.2

[ujmujm]

I'm machining a part on a Matsuura MX-520 and I need to probe a feature, I read the post (probing under G68.2) but I'm sorry I'm still lost! I thought it would be a piece of cake, but I'm really struggling. there are 8 holes total with a positional tolerance of .001  4 holes at .1235Ø and 4 at .0789Ø the inside of the slot walls are the datum's for the adjacent holes, here's my order of operations:

1) Block laying flat A,0 C,0 face the top walk around perimeter while holding onto the work stud on fixture.

2) Rotate part A-90° C90° mill slot.

3) Rotate part A-90° C180° probe wall of slot  and drill .079Ø hole.

4) Rotate back to A,0 C,0 and drill .1235Ø.

See attached PDF drawing Part2.PDF

 

 

[Guest]

So, are you needing to know what the code should look like when probing while TWP is active?

[Guest]

Can you share the CAD?

[ujmujm]

I created a cad file so I could make the attached PDF. that represents the part I'm doing, I'm not able to share the original cad file.

[Guest]

Probing with TWP is really no different than probing without it. Often I will use part's Datum in the orientation that makes sense and all my positions are relative to that position.

[crazy^millman]

Are you looking to use a 3 point or 4 point circle probing routine? Are you using the Renishaw or Matsuura Probing codes to prob the features? Foghorn teaches this to customers on a regular bases so you are in good hands if you can get him some specific information.

[ujmujm]

One of my attempts look something like this.

Working from my original WCS (G54)

G0 G90 G54 A-90.0 C-180.0
G68.2 X0.0 Y0.0 Z0.0 I-180.0 J-90.0 K0.0
G53.1
X-0.336 Y-0.098 A-90.0 C-180.0 

G65 P9810 Z-.118

G65 P9125 A8. S3. Q.75 (Probes "Y" )

G65 P9810 Z.2

G69

G53 Z0.

after I probed a new "Y" offset the tool went in the positive direction towards the top of the table. which made sense because my "Y" is now my "Z" and my "Z" is now my "Y" I've called Matsuura and I called the company that installed our Renishaw probing software and they really couldn't help me with working in a tilted work plane, the Renishaw programming manual has one page on working in a tilted work plane but it wasn't very helpful it mentioned a G53.6 instead of a G53.1 to align the tool posture to the active "Z" but I didn't have any luck with that.

 

[Guest]

G53.1 is correct.

Before the G65 P9810, you need to orient the probe and turn on the probe (under normal situations, unless your MACROS have been customized to turn it on with the G65P9810.

In my experience, the Easy-Set cycles don't work very well while in-process. So, I would change the G65P9125 to G65P9812 (single surface  probe cycle), and use the appropriate arguments. Unless you're measuring a posket in which case, go with a G65P9812 and the appropriate arguments.

You DO need to know an approximate position beforehand (i.e. have a rough work offset). Otherwise, MDI and Easy-Set to get you going.

HTH

[ujmujm]

Unfortunately we didn't get the Matsuura Renishaw probing we have the Renishaw macro's with a main template that points to the macro's

I have thirty parts to make out of 15-5PH with a tight positional tolerance on the eight hole's so I wanted to incorporate into the program to probe the side of the slot to put in the .0789Ø then rotate and put in the .1235Ø my new offset is G56 so I copied my "X" and my "Z" offset from my G54 and I was going to probe "y" every part should be able to meet that tolerance easy that way.

[ujmujm]

My O9812 macro is a web pocket measure. my templates main program looks like this, I was using N8 (Y NEG. SURFACE)

%
O2010(EZSET TEMPLATES PROGRAM)
G91G28Z0
 
(LISTING OF CYCLES TO SEARCH FOR)
 
(N1  BORE MEASURE)
(N2  BOSS MEASURE)
(N3  ID GROOVE-POCKET)
(N4  OUTSIDE WEB/RIB)
(N5  X POS. SURFACE)
(N6  X NEG. SURFACE)
(N7  Y POS. SURFACE)
(N8  Y NEG. SURFACE)
(N9  Z SURFACE)
("Q" IS ADDED SEARCH DISTANCE)

[crazy^millman]

I with Foghorn I would old school it and make sure you do the complete process. Once you call the probe the right way and get it where it should be then you should be off to the races. Do a search on the forum I shared a drill cycles process to make all the Renishaw probing cycles work with the Mastercam drilling cycles. I also liked to apply mt changes and go back and check things where were I thought they should be before cutting a part. Never hurts to check something twice and cut it once.

[ujmujm]

Actually that is what I was doing I created a tool using lollipop to my probe spec and then did a drill canned cycle  and modified the code when I posted it out worked great until my spot drill was off in the "Y" about eight inches, it seams so simple but I'm just not seeing it.

[crazy^millman]

How are you updating the workoffset? I have to break out my probing stuff, but I think it is S and are you updating the active offset or are you updating a common one and then doing the math from the active to the common to work out the difference of the G68.2 shift that is active? I have to suspect you don't have the right plane called or active the correct way when you are applying the results since you are in a G68.2 plane those values have to be accounted for. If they are not then you will be off a considerable distance.

[ujmujm]

I need to probe and install the .0789Ø then using tilted work plane install the .1235Ø that is perpendicular to it, just for kicks I tried putting the holes in without the G68.2 and the .0798Ø was within .0001's of the slot wall but the .1235Ø was a couple of thousands from the .0798Ø which was way out of tolerance. That did show me how accurate tilted work plane is though!

[Guest]

One single offset relative to the Datums in Top View is how I would do it. Multiple offsets complicate matters unnecessarily IMHO.

[ujmujm]

What you are saying makes sense at first I was just kind of poking and hoping, I was using active work offset (G54) to get the part rotated into position then I shared the "X" and "Y" from my G54 offset in G56 and probed a new "Y" and when that didn't work I used my active work offset to rotate the part into position and probed a new "X" , "Y", "Z" and stored it in G56 that also didn't work.

[ujmujm]

Your absolutely correct, I totally agree with what your saying, I have a situation that is out of my control though, the stock was ordered and the job was processed with the part laying down so I can only do four holes in the first operation and the other four in the second operation and the slot is .525 wide and 2.00 inches deep and the bottom of the slot is actually a pocket with 1/16 corner radii sounds like fun doesn't it, I ran 11 parts and 4 of them where to print the other 7 where out by .0005 to .0008, if  the width of the slot varies more than a few .0001's then my .001 positional tolerance is out. That's why I wanted to probe each set of holes, the wall of the slot is a datum and the center line of the .1235Ø is a datum.

[Guest]

Can you create a block with the same overall dimensions, then just create a point where two or 3 datums intersect?

[Guest]

The main thing to remember with TWP is that X0 is still X0, Y0, is still Y0, and Z0 is still Z0 no matter your position and orientation. So, in your case you need to adjust the work offset based on the error because your stock came in different than expected. So, you'll get yourself into position, measure the feature, capture the error amount do something like

#5221=[#5221+#140] (G54 X Work Offset Position Correction)

#5222=[#5222+#141] (G54 Y Work Offset Position Correction)

#5223=[#5223+#142] (G54 X Work Offset Position Correction)

Or whatever Offset you're writing to...

 

Make sense?

[ujmujm]

Thank you for your help, the Matsuura is a new machine tool for us, we've had DMG Deckel Maho's for ever which are a lot different, there tired though so the  powers that be would like to replace them with the Matsuura's looks like we are going to need a lot more training!

[Guest]

You're welcome. Training is always a good thing especially with a new machine. Do you use CAMplete with yiur new machine?

[ujmujm]

Yes we do, I'm going to get a quote from my reseller for a post  I'm not a big fan of Camplete.

[Guest]

Can I ask why you'te not a fan?

[crazy^millman]

44 minutes ago, ujmujm said:

Yes we do, I'm going to get a quote from my reseller for a post  I'm not a big fan of Camplete.

CAMPlete is awesome I think you need some training. You are going to throw away your insurance policy for crashing the machine to use a process that can crash your machine? I would like to know why also?

[ujmujm]

I've always used verify in Mastercam it's never let me down, I'm primarily a mill guy and CAMplete has been kind of a hassle, I love learning new things but I need to see value in it.