Printable View
I am working on a Haas VF5 with an indexable table. It has the inspection + software for the reinshaw probe. What i am looking to do is take two points one at the first point of the toolpath and one at the last point in the toolpath. From these two points i want to adjust the whole toolpath. Is this possible between haas and the reinshaw software? Still new at this so any help is appreciated
You should be able to do what you are asking. The Renishaw system should have come with a programming manual. Go through it and you should see an example similar to what you are asking along with many other routines.
If you do not have the manual, go to the Renishaw website and download it.
Also, if I understand your question correctly, you will need to make sure your machine has rotation and scaling option enabled.
Another question:
If i take the first and last point of the toolpath with the prob. Is there a way to just offset the first and last point and have all the points in between recalculated. Or will i have to take the 2 probe points find the degrees shifted from cad model and adjust this using a g19 g68 to rotate the part. with the g68 this will offset all points to this new angle. After that i will have to take the 2 points again find the difference between cad and what was read. then add these two together and divide by 2 to get the average. This will be put into the z to offset the tool.
let me know if this doesnt make sense.
No, I am not 100% clear what you are trying to accomplish.Quote:
Originally Posted by Iggyg00
Do you have a manual? Did you read it? If you answered no to any of these, then get the manual. It has a ton of information and will answer many questions.
If you still have questions after reading the manual and trying the routines, then come back with specific questions.
I'm not clear either. By "adjusting the toolpath", are you meaning you need to move your work offset to adjust for random placement in a fixture? Or a casting that varies? Try explaining exactly what you are doing. Pictures of the part may help.
I am writing my programs to a new oem part in mastercam. The problem with the parts is that they have been warped out of shape due to heating and cooling effects in the turbine engine causing location issues on the machine. My thought was to take a probe hit where the tooling path starts and a probe hit where it ends since x and y are ok. From these 2 points creating some sort of macro that will adjust the whole toolpath in space without having to modify the whole toolpath. Example is below....
Below is the code :
N180 X-24.8787 Y.1921 Z3.3043 F4.5 ( take hit on part at this location replace z)
N190 X-25.4262 Y.6322 Z3.1743
N200 X-25.9719 Y1.0726 Z3.0365
N210 X-26.302 Y1.34 Z2.9491 (take hit on part at this location replace z)
From those 2 hits N190 and N200 will be shifted in z automatically.
My only other option I think is to take hits at all z points so (n180, n190, n200, n210) and have those values replace the original this would correct the toolpath
Ok, so this is like a chamfer or ball nose or engraving toolpath, yes? To update all four spots in Z, this is what I would do:
M6 T25 (PROBE)
G43 H25
G65 P9832
G54 G0 G90 X-24.8787 Y.1921
G65 P9810 Z3.4043 F300.
G65 P9811 Z3.3043 S2. (DUMP Z LOCATION TO G56)
G0 Z4.
G65 P9810 X-25.4262 Y.6322 F200.
G65 P9810 Z3.2743
G65 P9811 Z3.1743 S3. (G57)
G0 Z4.
G65 P9810 X-25.9719 Y1.0726 F200.
G65 P9810 Z3.1365
G65 P9811 Z3.0365 S4. (G58)
G0 Z4.
G65 P9810 X-26.302 Y1.34 F200.
G65 P9810 Z3.0491
G65 P9811 Z2.9491 S5. (G59)
G0 Z5.
G65 P9833
G103 P1
#800=#5263 (#800=G56 Z)
#801=#5283 (G57)
#802=#5303 (G58)
#803=#5323 (G59)
G103
(TOOL CHANGE AND WHATEVER COMES BEFORE N180)
N180 X-24.8787 Y.1921 Z#800 F4.5
N190 X-25.4262 Y.6322 Z#801
N200 X-25.9719 Y1.0726 Z#802
N210 X-26.302 Y1.34 Z#803
Run this code at your own risk. I have no idea what kind of obstacles the part presents.
EDIT: If you were to only check two points, you could average the error between nominal and actual, then update your work offset with that result, but how are you to know if all the points in between fall on that average error?
Whoops. Meant to edit the above post, not make a new one. It's been a long few days. :)
Quote:
Originally Posted by Iggyg00
Quote:
Originally Posted by Matt@RFR
My point exactly!
How would you expect the machine to "automatically" know how much to shift all the points in between?
How would you expect the machine to "automatically" know how much to shift all the points in between?
that was what i was trying to figure out.
The probing routine is the best option i think as all z points in the program can be replaced.
THANK YOU ALL FOR THE HELP!!!!! know its time to head out to the machine and try some things.
Uh. Can I get the numbers of the planes these turbine engines are going on?Quote:
Originally Posted by Iggyg00
dont worry txcncman they dont go in the air..... This is not dimensional machining of the part. This is used after the parts come in from being engine run to cut off sheetmetal parts from the casting to save and reuse. I am only trying to cut welds and not base metal from the part.
Whew! Thanks. I feel a little better now.