dstryr
Diamond
- Joined
- Jan 22, 2010
- Location
- Nampa Idaho
Anyone here have it and played with it a bit? Got it working today and messing with it. Cool software. Just eats up a lot of time running, moving, thinking, re run, repeat.
Follow along with the video below to see how to install our site as a web app on your home screen.
Note: This feature may not be available in some browsers.
Largest Manufacturing Technology Community on the Web
Stay Connected:
Renishaw Axiset
- Thread starter dstryr
- Start date
- Replies 18
- Views 6,716
Mike1974
Diamond
- Joined
- Nov 5, 2014
- Location
- Tampa area
I just looked at the video on their website, looks pretty cool. Our HaasUMC750 came with something like this. It is a sphere mounted on a shaft at 45deg, similar to what is shown in the video, except larger. I have not used it yet, I just watched the setup guys run through it. It runs just like a probe cycle inside the VQC. I think (again I have not done it myself) I record some numbers in the parameters and then run the test cycle and compare them. If they are off by more than whatever the standard deviation is I need to make a correction in the parameters.
Does this software do something similar? I see in the video it outputs information, but how do you fix it if the numbers are very bad? Is it just a checkup tool so you can call a tech and then they come do the work on the machine? Do other machines have a similar offering as Haas, supplying the test sphere and program to do a self diagnosis?
Does this software do something similar? I see in the video it outputs information, but how do you fix it if the numbers are very bad? Is it just a checkup tool so you can call a tech and then they come do the work on the machine? Do other machines have a similar offering as Haas, supplying the test sphere and program to do a self diagnosis?
TeachMePlease
Diamond
- Joined
- Feb 11, 2014
- Location
- FL
Funny, I just watched the video of that probing routine in the UMC750 on youtube last night. Looked pretty damn cool. Do be sure to post a review of the machine after you've run it for a bit. It was a neat looking piece of kit, for sure.
dstryr
Diamond
- Joined
- Jan 22, 2010
- Location
- Nampa Idaho
It outputs data which allows you to import into a computer and see whats going on with the data points. After you see what is off it is clear what needs to be adjusted. The software will autoadjust but the adjustment isnt always clear and dry. Sometimes its a pivot point adjustment, other times its the center of rotation adjustment. I spent about 4 hours using it on both of my machines yesterday. Going to cut some parts later this week that will show me if I'm any bettter than when I started.
Reason I bought it was because I'm always fighting blends between the bottom of endmills at a0 and the side of ball endmills at say a-45.
To Dennis
What I do is spot a feature that should be in the same position from c90 and c270 once you find your center between those two sides I use separate offsets for c180 c0 sides. I try to use the side of end mills at "a0" generate the profile of the part this is my g54 =a0. Than when you rotate down to g55 a90 those walls will always be square and parallel. So if a0. = g54 = 1.337degress a90.= g55= 1.337 + 90. Than adjust x at g54 for true center along with y and move g55 x to center of runout when rotating c axis.
I know there's a lot of parts that have to use the bottom of endmill at a90 because of tight radii that need ball mill surfacing and such but I always try to use the side of endmill even at a90. Profile at c0. Rotate to c90. Profile again to generate than when you put a feature inside that side milled profile it's easier to spot where your off...you eliminate the tool length and know it's the work offset...
I always knock my fixturing on center in a trunnion rotations the c axis indicating a know bore or boss on fixture that way your not running out less than a half thou to a tenth or two. I also jog tools into material and rotate c to make a boss and than indicate that. Most of my
Work is from bar and done part off complete minus one dim that can be land on a second op. Second ops on fixturing that doesn't repeat with corner rounders and ball milling on two opposite sides of the part is always fun
What are your practices for programming to establish true datums
And trapping dims on your 5 axis positioning work?
What I do is spot a feature that should be in the same position from c90 and c270 once you find your center between those two sides I use separate offsets for c180 c0 sides. I try to use the side of end mills at "a0" generate the profile of the part this is my g54 =a0. Than when you rotate down to g55 a90 those walls will always be square and parallel. So if a0. = g54 = 1.337degress a90.= g55= 1.337 + 90. Than adjust x at g54 for true center along with y and move g55 x to center of runout when rotating c axis.
I know there's a lot of parts that have to use the bottom of endmill at a90 because of tight radii that need ball mill surfacing and such but I always try to use the side of endmill even at a90. Profile at c0. Rotate to c90. Profile again to generate than when you put a feature inside that side milled profile it's easier to spot where your off...you eliminate the tool length and know it's the work offset...
I always knock my fixturing on center in a trunnion rotations the c axis indicating a know bore or boss on fixture that way your not running out less than a half thou to a tenth or two. I also jog tools into material and rotate c to make a boss and than indicate that. Most of my
Work is from bar and done part off complete minus one dim that can be land on a second op. Second ops on fixturing that doesn't repeat with corner rounders and ball milling on two opposite sides of the part is always fun
What are your practices for programming to establish true datums
And trapping dims on your 5 axis positioning work?
Hansdie
Hot Rolled
- Joined
- Jul 21, 2005
- Location
- San Francisco, CA
Heidenhain has had this for 6-7 years its called KinematicsOpt.
HEIDENHAIN Places Machine Tool Accuracy On Center Stage at WESTEC
Before that, and still sometimes now, we used a Square block bolted to the table and a special macro for measuring points on the block
So your blends always come out perfect from your cam?
Hansdie
Hot Rolled
- Joined
- Jul 21, 2005
- Location
- San Francisco, CA
Depends on what the definition of perfect is but pretty close to perfection.
Within a thou would be my goal for positioning and dia perfect if the blends allow it but in tolerance is good enough... And I guess it matters if your starting from a blank or working off of a second operation...fixturing is mostly the limiting factor for me. You can't reinvent the wheel when the setup time says five hours.
Hansdie
Hot Rolled
- Joined
- Jul 21, 2005
- Location
- San Francisco, CA
couple tenths at most doesn't matter if we start out with a blank or second op we can realign off of planes and cylinders.
dstryr
Diamond
- Joined
- Jan 22, 2010
- Location
- Nampa Idaho
Yup. This is what I was aiming for. It is always a problem with cutting a flat floor at a0c0 and then trying to blend up to the floor with a ball at say a-45 c0. Usually its like the tool or the y is off about .001-.002. The axiset showed me that my Y Z pivot point over the A axis was off .001 in both directions, oppposite from each. This correlated what I've seen when cutting parts. I will know for sure tomorrow when I get back to another complicated job.
Handsie you have hermle and I have ....well you know. Not a fair comparison
.dstryr
Diamond
- Joined
- Jan 22, 2010
- Location
- Nampa Idaho
*Update*
Used this on both 5 axis machines. Blends are down around .0005 now. The rest I'm sure is tool length offsets and a little bit of spindle growth. Happy Customer!
Parts from this last batch after using the Axiset look a lot better and take a lot less hand work.
Used this on both 5 axis machines. Blends are down around .0005 now. The rest I'm sure is tool length offsets and a little bit of spindle growth. Happy Customer!
Parts from this last batch after using the Axiset look a lot better and take a lot less hand work.
PROBE
Hot Rolled
- Joined
- Jan 23, 2003
- Location
- Tel Aviv, Israel
The mentioned pivot point and center of rotation adjustment - which Fanuc parameters are updated ?
Mike1974
Diamond
- Joined
- Nov 5, 2014
- Location
- Tampa area
RE my post I made last year. I have ran the cycle twice now for my UMC750. I only saw a few tenths (actually measured in encoder counts) variation between both times I ran it and the original setting from when the machine was set up. Quite surprised the machine did not move around after it had settled.
LockNut
Stainless
- Joined
- Jan 6, 2007
- Location
- Bergen County
dstryr
Diamond
- Joined
- Jan 22, 2010
- Location
- Nampa Idaho
Sorry machine is Siemens control
PROBE
Hot Rolled
- Joined
- Jan 23, 2003
- Location
- Tel Aviv, Israel
Thank you.
PROBE
Hot Rolled
- Joined
- Jan 23, 2003
- Location
- Tel Aviv, Israel
I've been approached by customer with substantial number of 5 axis Makinos A51 ans Matsuuras MAM72 to supply the system to solve the problem of kinematic discrepancies. As machines are equipped with standard touch probes from several suppliers and not Renishaw Rengage, the use of Axiset wasn't the option.
I wrote the routines, which execute the measurement of calibration sphere in bunch of B and C axis positions. All calculations are made in macro (no need to use external PC), at the end the 19700-19705 parameters are updated, or alarm is raised if mechanical intervention is needed.
Now I would like to understand how these parameters are executed. Should X and Z axes move when B axis (primary rotary)is rotated ?
I wrote the routines, which execute the measurement of calibration sphere in bunch of B and C axis positions. All calculations are made in macro (no need to use external PC), at the end the 19700-19705 parameters are updated, or alarm is raised if mechanical intervention is needed.
Now I would like to understand how these parameters are executed. Should X and Z axes move when B axis (primary rotary)is rotated ?
