Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Haas UMC 750SS


Recommended Posts

  We bought a new Haas UMC 750SS. Its been a nightmare. Nothing was accurate or even repeatable. Its been leveled 4 times. They have completely remapped the rotary and linear axis's. The supposed final fix was Haas leveling the machine in a non-standard way. They used the probe and inspection balls to level the machine. In my opinion they twisted the machine until it gave good number. 

So yesterday we tried to use the machine and by the end of the day the Z value of the tool was off a quick check shows my Haas factory gage tool showed it was off .0012" when using the touch setter. The touch setter was set that morning using that tool to zero it. Now the air temp in the room did get warmer as the day when on, less then 20 degrees change. Some here think that is why its off. To me 20 degs should not equal .0012 variation. Also the machine has a thermal  growth sensor for the Z. What do you guys think? any experience with a UMC 750 out there? I will be talking to Haas but the owner is at his end with this machine. Its been sitting on our floor since early November. So far all its done is rough about 20 parts. The worst part is its a pallet pool system he had planed on running 24 hours a day. 

 

  

Link to comment
Share on other sites

Absolutely stinks!

Sorry I have nothing to add but only to say, I have heard this about these machines from several people I Know...one went so far as to send the machine back.

Good luck, hope they can figure out something that works for you.

Link to comment
Share on other sites
1 hour ago, DC Gorn said:

Some here think that is why its off. To me 20 degs should not equal .0012 variation.

Haas Z axis are notoriously unstable. I am running an UMC 750 and the spindle often grows 0.002 through the day. 

  • Like 1
Link to comment
Share on other sites

I ran a VF-3SS with a trunnion for six years.  The Z would move about .0015" over the first couple hours of running in the morning, and that was in a +/- 2°F environment.  20° is a wild swing.

Technically they do have thermal comp, but from what I hear it doesn't work very well.  If you need better than that level of accuracy you'll have to control the temp tightly, program automated probe and adjust routines, or just program to automatically touch off every tool at it's picked up.

  • Like 1
Link to comment
Share on other sites

I have it from a reliable source that the main problem is that Haas has multiple parts sources.

When you by a Mori or Matsura or other primo machines they have one type of widget, which has been selected specially to work well with all the other widgets.

Haas sources the same widget from multiple companies and throws them in a big box in assembly, so the system is not as tightly regulated and also not as "tight".

Link to comment
Share on other sites
23 hours ago, nickbe10 said:

Haas Z axis are notoriously unstable. I am running an UMC 750 and the spindle often grows 0.002 through the day.

 

So with the pallet system the owner want to run lights out on Aero Space parts. You think if we ran continually it would normalize? Since the touch setter seem to see the same error as the part what would you think about touching off critical tools before running them each time?   

I was aware of the rotation accuracy but I was told that it was repeatable. But Haas advertises .0002" Accuracy and .0001" repeatability on linear axis's.  We where told the UMC 750 went through a redesign just a few years ago to improve accuracy. Since we are looking a production repeatability is by far the more critical of the two.   

I did not mean for this to be a Haas bashing thread. I was assuming there was something wrong with this machine. My only experience with Haas has been the 5 axis VF2 cutting Aluminum.  I do miss my DMU 70 heck even my Variaxis i700.  

Link to comment
Share on other sites
20 minutes ago, DC Gorn said:

So with the pallet system the owner want to run lights out on Aero Space parts. You think if we ran continually it would normalize? Since the touch setter seem to see the same error as the part what would you think about touching off critical tools before running them each time?   

I was aware of the rotation accuracy but I was told that it was repeatable. But Haas advertises .0002" Accuracy and .0001" repeatability on linear axis's.  We where told the UMC 750 went through a redesign just a few years ago to improve accuracy. Since we are looking a production repeatability is by far the more critical of the two.   

I did not mean for this to be a Haas bashing thread. I was assuming there was something wrong with this machine. My only experience with Haas has been the 5 axis VF2 cutting Aluminum.  I do miss my DMU 70 heck even my Variaxis i700.  

+/-.005 Aerospace maybe, but tight tolerance parts expect problems. Need to use probing and a standard monument feature on each part to use to gauging. It could be a tooling ball or a gauge block that will allow you to check something that should never change in size to gauge deviations and then program in a way that compensates when the measurement of them changes.

  • Like 1
Link to comment
Share on other sites
17 minutes ago, DC Gorn said:

I was aware of the rotation accuracy but I was told that it was repeatable. But Haas advertises .0002" Accuracy and .0001" repeatability on linear axis's.  We where told the UMC 750 went through a redesign just a few years ago to improve accuracy. Since we are looking a production repeatability is by far the more critical of the two.   

To be fair I interpolate holes to =/- .0001- .0002, so they are just being a bit economical with the truth.

Re-probing and re-touching critical tools, might help, but I might be tempted to run Productivity+. Then you can probe for stock.

This might also require re-calibrating the probe. Contact Renishaw for the straight skinny on this, I have always found them to be very straight forward.

Monitoring your spindle growth through the process might just do the trick as well. Once the spindle grows, does it stay there for the rest of the shift? As long as you don't shut it down too long before starting the unattended work you might get away with it.

 

  • Thanks 1
  • Like 1
Link to comment
Share on other sites

It will be more stable if you keep it running nonstop, and if you can manage your HVAC situation.  Probing each tool as you pick it up will also help.  Don't rely on the Z of the spindle probe; that will move with your thermal growth.

Here's another idea, kind of similar to Ron's.  When I'm picking up the Z of the center of rotation of a trunnion, after getting it close, I'll tilt over 90°, cut a face, spin 180°, and cut the opposite face.  Then I can mic between the faces to gauge my error, and adjust that out.  You could automate that at the start of your part, and instead of micing, tilt back to 0° and probe in X.  Then a simple macro can fine adjust your Z for every part.

  • Like 1
Link to comment
Share on other sites

We had a similar issue on a UMC-1000 recently, and while I can't reveal any customer specifics, here is how we addressed the issue:

  • Testing revealed that Thermal Compensation was continuing to add growth over time, even though the growth had stabilized.
  • We worked with the Haas Factory to generate a "Patch File", which disabled the Thermal Compensation feature. (I'm not 100% sure if it disabled all thermal compensation, or just disabled the sensors on the Spindle Cartridge.)
  • Due to turning off the Thermal Comp, it was necessary for the customer to run a modified Spindle Warm-Up program. We extended the length of the warm-up from 20-minutes, to 30-minutes, and added code to "stroke the XYZ and B/C Axes", as we ramped up the spindle to full RPM over 20 minutes, and then ran at Max. RPM for 10 minutes.
  • Once the warm-up cycle was complete, we then performed a full calibration of the Tool Probe, and then touched off all tools for a given job. (Must measure the tools with the spindle in the "warm state".)
  • With the machine warm, we then calibrated the "Spindle Probe Length" (Z calibration).
  • Then we calibrated the Spindle Probe Diameter, using a Ring Gauge.
  • Finally, we ran the Axiset Macros for the B-Axis, and then ran the Axiset Macros for the C-Axis. (There are two sets of macros when using the Renishaw product. This is not the same macro package as "MRZP Calibration", that come installed with the machine.)
  • When running parts, we use the Spindle Probe to pick up the Work Offset (Program Zero), G54 (or G55, or G56, Etc.)
  • For critical location features, it is beneficial to use Spindle Probing, to pickup a local work offset for adjusting critical features. So even though we use DWO/TCPC for most features, if you have a critical "True Position Tolerance", your most reliable solution is to perform "in-process Probing", using a local Work Offset for that feature. To do this, we typically use G55, or G56, etc., and have code at the top of the program which simply assigns those values to equal "G54 Offsets", after we have finished probing to pick up the current location of G54 on the individual part being run.

By disabling the Thermal Compensation with the Patch File, it then becomes necessary for the customer to use "process techniques" to manage the Thermal Growth, and it becomes critical for the customer to "not cut parts until the machine is fully warm".

I would also suggest checking with your HFO & the Haas Factory, to ask if these Thermal Compensation issues are being addressed in current or future software release.

And please do me a favor, and don't start the conversation with "Well Colin Said...", as you may be experiencing a different Thermal Growth issue, but this sure sounds a bit similar to the issue we dealt with recently.

However, I don't speak officially for Haas on this issue (as I don't think you're one of our customers, and unless Phillips is your HFO, I don't have authority to speak on this officially), so please just treat this information as anecdotal, and see if you can get your HFO to request a Patch File, to disable the Thermal Comp.

That will at least stop the control from applying a "growing comp value" to your machine. But you will see a difference in cutting, between a warm machine, and a cold machine, by disabling the Thermal Comp. However, if you know how the machine is going to behave in certain environmental conditions, and you manage that thermal cycling of the machine properly, then you will be able to achieve consistent performance.

But I would strongly recommend integrating Spindle Probing into your machining processes, both for locating each part prior to machining, and also for hitting any critical tolerance features, by performing in-process probing, and adjusting the individual coordinate system values for "each critical feature or face".

You mentioned "Haas advertises 0.0002" accuracy, and 0.0001" repeatability". Do you have a document or web link that shows this?

https://www.haascnc.com/service/online-manuals/umc-series/umc---geometry.html#:~:text=It%20is%20important%20to%20remember,accuracy%20is%20%2B%2F%2D%2015%20arc.

According to Tab 7.3 GEOMETRY - TROUBLESHOOTING:

It is important to remember the Linear accuracy of the machine is 0.0004/10" and the angular accuracy is +/- 15 arc. sec. These tolerances can add up quickly.

The 5-Axis machines are never listed as a overall static accuracy across the entire linear stroke. As you can see above, the specification is 0.0004" over 10 inches, not over the entire travel range. And, you have +- 15 Arc Seconds of Rotary Positioning accuracy. Like a "wedge of pie", the farther you are cutting away from the rotary centerline, the more those angular errors are magnified as a linear distance. Also, the "table weight" becomes a concern for large part/fixture combinations. If you are cutting a 20" diameter part, that linear accuracy is more like 0.0008" over that distance. Now, that is the specification, and we can often achieve much better tolerances. I've personally seen most of the UMC-750 machines hold more like 0.0002-0.0006", over a 25" long part. But, that is also the 'dynamic accuracy', so with adjusting cutter compensation, using probing, and other "process techniques", we can get down closer to the lower end of that tolerance range, when it comes to repeatability.

 

  • Thanks 1
  • Like 2
Link to comment
Share on other sites

The other thing to understand, is the difference between alignment of the machine geometry and machine leveling, and setting > Center of Rotation Parameters. That isn't leveling, and it doesn't twist your machine. When you mention "Probe and Inspection Balls", you are talking about the MRZP Process. This sets the Machine Rotary Zero Point.

Depending on your software, and which Macro Programs you are running, this either sets Settings 254-257, or Settings 300-305.

These values are used with a combination of the following:

  • Accurately measured TLO values (positive Tool Length Offset values)
  • Accurately measured Work Offset Location. Do not use "Centerline of Rotation" for your Work Offset. The number of people I have seen, who insist it must be done this way, is staggering. Make the location for your Work Offset, a feature on the part or fixture which is easy to PROBE. Preferably, a location on the Part itself.
  • Accurately set MRZP Values. The 'Renishaw Axiset Macros' do the best job here. Talk with your HFO about getting these macros loaded. From what I've been told by Renishaw, we are allowed to install and run them on a UMC where the customer has not purchased the Axiset package, however we are not allowed to supply the Excel Spreadsheet which comes with the package, and is used to track geometric values over time. (To help you track the dynamic performance of the machine.) These Axiset Macros are especially good at finding the "offset" for the C-Axis Platter. This is Setting 254.
  • Settings 255-257 describe the "centerline of the B-Axis" from Machine Zero. Setting 254 is the offset (+-) from this centerline position (along the X-Axis), for the center of platter (C-Axis) rotation. The note on the screen says "should be no more than +- 0.005", but I have seen that value up to 0.0087" > and the machine cut very accurately on a full 5-Axis Part, because we accurately measured "the true state of the machine".
  • You MUST, MUST have a Post Processor which invokes both DWO (G254) and TCPC (G234) codes, in the proper way.
  • This means you must be sure DWO & TCPC are properly canceled, between Ops, especially if you are changing modes.
  • You must call the Active Work Offset (G54 typically, but could be any of them), Position the Rotaries (B & C move), and then call either DWO or TCPC Codes.
  • TCPC must start with a G0 move, and you typically need to "recall the current position on the G234 line".
  • For TCPC, I prefer to have a "prepositioning move" done using DWO, so the tool can approach "from the correct direction", cancel DWO, and then invoke TCPC.

None of those Machine MRZP Values are used, if you aren't invoking DWO or TCPC.

Let me state that again > none of those Machine MRZP Values are used, if you aren't invoking DWO or TCPC  and calling it properly!!!

If you are just using Work Offsets (G54, G55, G56, Etc.), and programming from COR of the machine, then you're not utilizing the power of the machine. If you aren't integrating Probing into your processes, you're not utilizing the power of the machine, and you're going to have difficulty using that Pallet Pool, because you need to be able to account for the variations of each pallet/part. You do this with a Probe, not with "a perfect setup". There is no such thing as a "perfect setup", unless you're in a Laboratory. When I worked at Methods Machine Tool, we had a lab for our Yasda machines, where the temperature did not vary more than 0.5 degrees C (1-degree F), over a 24 hour period, and the entire volume of air was replaced every 3 minutes in a 3000 Sq.Ft. room. We still used a Probe, but we were able to hold +- 1 micron on the PX30i (production machine), and we were able to split a Micron (+- 20 millionths), on a YMC650. Each machine was also placed on a 40" thick isolated and reinforced slab, with 5000 PSI concrete.

That said, when a Haas machine is calibrated properly, and you're using the Probing System for critical features, along with Probing your Tool Length, and Probing Parts for Work Offset Location, you should get incredible performance from your UMC-750SS with Pallet Pool.

Are you using High Speed Machining? Are you adjusting your G187 P values (P1-P3) to switch between Roughing and Finishing Mode? Are you setting the Corner Rounding value with the E parameter?

Rough = G187 P1 E0.04

Semi-finish = G187 P2 E0.004

Finish = G187 P3 E0.0004 (sometimes I drop it to E0.0001).

Are you using "Exact Stop" for Drilling, Reaming, Boring? (G61 > Exact Stop Mode, G64 > Normal Machining Mode, or place an individual "G9" on each line of your Canned Cycle. You can use G9 to enable "Exact Stop" for individual holes. So if you were spot drilling 10 holes, and 2 are dowel holes, you could place a "G9" on those two holes only. NOTE: you will get a slowdown when using Exact Stop, but the locations are more accurate.)

 

 

  • Thanks 1
  • Like 2
Link to comment
Share on other sites

I do, but I work for the Federal Division, however I know the Applications Manager for Phillips Commercial quite well. Please PM me your Serial Number, and I'll touch base with my counterpart in the Commercial Division, and we'll get you the Service/Support you need.

To be fair, it sounds like there is also an opportunity for both Applications & Probing Training at your company, because "Probe Calibration" is a process you should know intimately. I would suggest that you'll want to calibrate weekly, until you really get the hang of the process.

You may even want to spend a full day where you cut-and-test to get some data. Start by "calibrating at the low air temperature (after warming up the axes & spindle) first thing in the morning" (record all values), and then perform that same "full calibration process at Noon" - recording all data, and do a final calibration at 4-or-5 PM. What we are after here is "how much influence does the thermal cycle have on the process". 

As I mentioned, it takes process knowledge and Probing to really get the full capability of these machines, in addition to a properly formatted Post Processor. Things like using the High-Speed Codes, proper use of TCPC & DWO, and in-process Probing for those high-accuracy applications, are all critical to holding super tight tolerances.

I have setup a process (funnily enough, on a Pallet Pool, just not a Haas Pallet Pool), that performed "full Calibration" before each part was cut. This allowed us to hold very tight tolerances, even as the machine warmed up from cold (cycle time was about 18-minutes). I don't believe you'll need to go to that extent, but it always depends on the part size, material, tools, fixturing, and thermal stability of the shop in question. In this case, performing the calibration (tool probe & spindle probe), then measuring the tools, and then probing the part which was freshly loaded into the machine, gave us the ability to hold some very critical in-line bore tolerances and true position locations, for some Port Features.

I could not have done that using the static accuracy of the machine, throughout the thermal cycle of daily production. Without the Probe, I would have been chasing offset adjustments all day, and scrapping parts. By integrating the Probe into the process, not only did I hold tolerance, but setups became a lot less fussy. I could simply clamp parts in a fixture or vise, without stressing over trying to get those OP20 Parts precisely on location. I could measure each part "in the location it was at", without worrying if each pallet was built or setup precisely like the other pallets. This vastly simplifies your setup, because it just doesn't matter if you are slightly out of position, so long as you "probe that error", and correct the twist or positional error using your C-Axis Work Offset value. (NOTE: you must correct any C-Axis Error, and recall the work offset, and C-Axis (zero) position, before Probing for XYZ translation error). But you should also be aware of this limitation on the Haas > the DWO Function only compensates for single "rotary axis errors". So you can correct a C-Axis misalignment, but not a B-Axis error.

So what I mean to say there, is that you shouldn't be sloppy with your fixture setup/building. If possible, machine soft jaws, or the mounting surfaces of your fixture "in place, on the machine", so the fixture is as precise as you can get it. But when you mount parts, if you incorporate the Probe into the mix, you don't have to be as careful in setting up the parts for XYZ location, but you should still be careful, as some rotary error cannot be corrected for using the DWO Function. (Fanuc WSEC Function allows 6-degrees of freedom correction for errors.)

  • Thanks 1
Link to comment
Share on other sites

FYI While I am not the best at the machine, more statistical processing and fixture design, we have others that are very good. We have 2 other % axis machines. Even with the Haas techs setting MRZP we where seeing .006" error.  Haas also sent in the equipment to remap the ball screws. 

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

×   Your link has been automatically embedded.   Display as a link instead

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×