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:

Mastercam 5 Axis


Sam1
 Share

Recommended Posts

  • 3 months later...

Sorry to resurrect an old thread but I'm digging around trying to find out why a UMC-750 sometimes slows to a crawl when doing five axis milling, even in G93.  Has the Haas got a reputation for slowing down when running five axis code (especially near B0)?  If so, was the UMC-750SS specifically developed to address this situation?

Link to comment
Share on other sites
On 10/2/2020 at 5:35 AM, Rstewart said:

That looks like one of the earlier models of the UMC.  They were pretty slow for sure, the newer ones do move a Lot more efficiently.

Yes did a turn key for a customer on a UMC-1000 with a Schunck Zero Point system last year. I was running 5 Axis at about 300 imp with no issues.

2 hours ago, Rich Thomas 4D Engineering said:

Sorry to resurrect an old thread but I'm digging around trying to find out why a UMC-750 sometimes slows to a crawl when doing five axis milling, even in G93.  Has the Haas got a reputation for slowing down when running five axis code (especially near B0)?  If so, was the UMC-750SS specifically developed to address this situation?

Rich we are not getting anywhere near B0 on thee toolpaths so I cannot say. Can the part be put on a riser or something done to get it a little further way from the Kinematic Zero? Is the post going high enough with inverse time? Has anyone tested how high a number the machine can have. Old Fanuc issue with inverse and Mastercam post comes to mind. Mastercam post limit inverse time to 9999 when most machines can handle 999999 for inverse time. Remember the higher the number to more it help with slower feed rates needed is certain areas. If the number is only getting up to 9999 and needs top get higher near B0 that could be the issue since inverse time is just that the inverse of what we think it should be.

  • Like 1
Link to comment
Share on other sites

Rich,

Does this machine have Haas High Speed Machining option? Is it enabled?

Also, contact your local Haas Service Provider, and make sure (doubly-sure), that you are running the latest Control Software version. (Most of the Haas Outlets will not want to update software, on a Milling Machine that "isn't having issues". However, there have been several updates to the Control Software for the UMC line of machines, and you want to be sure that you're taking advantage of all of those bug fixes and processing improvements.)

If it does have HSM, and HSM is active, change the Corner Rounding (Setting 85 or 191, can't remember which off-hand) to 0.02-0.04" (0.5-1mm). Then, try using a looser tolerance, with your vectors spaced a little farther apart.

Even with HSM option enabled, you'll be limited to about 80 Blocks per Second. So feeding the control "less vectors" is sometimes the answer, especially when roughing. When you are finishing, the feed rates are generally slow enough that you can use more vectors, as you aren't trying to "out-feed" the vectors as much at slower speeds.

Also, the "max Inverse Time Feedrate" is set, by default, at 9999.999, in most Posts.

The Max Inverse Time Rate on the UMC-750, is actually more like 40,000.0, so you should modify that parameter in the Post.

  • Like 1
Link to comment
Share on other sites
1 hour ago, crazy^millman said:

 

Rich we are not getting anywhere near B0 on thee toolpaths so I cannot say. Can the part be put on a riser or something done to get it a little further way from the Kinematic Zero? Is the post going high enough with inverse time? Has anyone tested how high a number the machine can have. Old Fanuc issue with inverse and Mastercam post comes to mind. Mastercam post limit inverse time to 9999 when most machines can handle 999999 for inverse time. Remember the higher the number to more it help with slower feed rates needed is certain areas. If the number is only getting up to 9999 and needs top get higher near B0 that could be the issue since inverse time is just that the inverse of what we think it should be.

 

I have a section of NC code below where the machine is moving very slowly:

N1542 X-8.4168 Y-2.1774 Z2.5202 B.4394 C-63.5988 F594695.09172
N1544 X-8.4159 Y-2.1778 Z2.5203 B.4049 C-67.425 F594695.09172
N1546 X-8.415 Y-2.1783 Z2.5205 B.3724 C-71.9412 F594695.09172

I'm not too clued up on Inverse Time feeds but a value of F594695 appears (to me anyway) to be a reasonable value over such small moves (plus this customer runs in inches) but the machine really slows down at this point.  At slower feeds, away from B0 the machine is moving faster over similarly short distances/angles.  

It may be possible to reposition the job but this a porting job on a car cylinder head and I don't think there is a lot of space to spare in the machine.  I don't want to go into detail in case I am being watched... but let's just say that "trial and error" doesn't go down well at this firm so I'm trying to pick off the low hanging fruit first!

Link to comment
Share on other sites
12 minutes ago, Colin Gilchrist said:

Rich,

Does this machine have Haas High Speed Machining option? Is it enabled?

Also, contact your local Haas Service Provider, and make sure (doubly-sure), that you are running the latest Control Software version. (Most of the Haas Outlets will not want to update software, on a Milling Machine that "isn't having issues". However, there have been several updates to the Control Software for the UMC line of machines, and you want to be sure that you're taking advantage of all of those bug fixes and processing improvements.)

If it does have HSM, and HSM is active, change the Corner Rounding (Setting 85 or 191, can't remember which off-hand) to 0.02-0.04" (0.5-1mm). Then, try using a looser tolerance, with your vectors spaced a little farther apart.

Even with HSM option enabled, you'll be limited to about 80 Blocks per Second. So feeding the control "less vectors" is sometimes the answer, especially when roughing. When you are finishing, the feed rates are generally slow enough that you can use more vectors, as you aren't trying to "out-feed" the vectors as much at slower speeds.

Also, the "max Inverse Time Feedrate" is set, by default, at 9999.999, in most Posts.

The Max Inverse Time Rate on the UMC-750, is actually more like 40,000.0, so you should modify that parameter in the Post.

Hi Colin, I'm waiting for the serial number from the customer so I can log a case with Haas UK.  I will ask them to check the status of the software on the machine.  I'm not sure at this point if HSM is active - again I'll be able to ascertain that once I get the serial number to Haas UK.

Setting 85 is 0.025" and 191 is set to "finish" which I think are good settings as far as I can see (and the custom is running in inches).  The 80 blocks per second is interesting though - we haven't tried looser spaced vectors yet.

We are seeing inverse time feeds of over 500,000 and the machine hasn't complained about feeds yet!  They are getting a "ROTARY AXIS COMMAND EXCEEDS PRECISION" error which might be down to the number of decimal places (four) in our rotary axis commands or maybe the rounding of the fourth digit.

 

 

Link to comment
Share on other sites
1 hour ago, Rich Thomas 4D Engineering said:

Hi Colin, I'm waiting for the serial number from the customer so I can log a case with Haas UK.  I will ask them to check the status of the software on the machine.  I'm not sure at this point if HSM is active - again I'll be able to ascertain that once I get the serial number to Haas UK.

Setting 85 is 0.025" and 191 is set to "finish" which I think are good settings as far as I can see (and the custom is running in inches).  The 80 blocks per second is interesting though - we haven't tried looser spaced vectors yet.

We are seeing inverse time feeds of over 500,000 and the machine hasn't complained about feeds yet!  They are getting a "ROTARY AXIS COMMAND EXCEEDS PRECISION" error which might be down to the number of decimal places (four) in our rotary axis commands or maybe the rounding of the fourth digit.

 

 

That all looks pretty good, except the "Max Inverse Time Value", which is way too high.

Try "medium" with Setting 191, which may help "open up the tolerance", if needed.

 

Rotary Axis Command Exceed Precision - That could be from the precision of the rotary axis NC Code "input", but could also be the Inverse Time Feed Values, giving a value that exceeds the Haas Maximum value on the control. 

 

Look at the English - Mill Operator's Manual (NGC 2020 Release).

Start at Page 233, and read to Page 247. I copied some information below:

 

 

Five-Axis Programming Notes:

Program approach vectors (moving tool paths) to the workpiece at a safe distance above or to the side of the workpiece. This is important when you program the approach vectors with a rapid move (G00), because the axes arrive at the programmed position at different times; the axis with shortest distance from target arrives first, and longest distance last.

However, a linear move at a high feed rate forces the axes to arrive at the commanded position at the same time, avoiding the possibility of a crash.

G-codes:

G93 inverse time feed mode must be in effect for simultaneous 4- or 5-axis motion; however, if your mill supports Tool Center Point Control (G234), you may use G94 (feed per minute). Refer to G93 on page 366 for more information. Limit the post processor (CAD/CAM software) to a maximum G93 F value of 45000. This is the maximum allowable feedrate in G93 inverse time feed mode.

Options Programming:

M-codes

IMPORTANT: When doing any non 5-axis motion, engage the rotary axes brakes. Cutting with the brakes off causes excessive wear in the gear sets.

M10/M11 engages/disengages the fourth axis brake.

M12/M13 engages/disengages the fifth axis brake.

When in a 4 or 5 axis cut, the machine pauses between blocks. This pause is due to the Rotary Axes brakes releasing. To avoid this dwell and allow for smoother program execution, program an M11 and/or M13 before the G93.

The M-codes disengage the brakes, resulting in a smoother and uninterrupted flow of motion. Remember that if the brakes are never re-engaged, they remain off indefinitely.

Settings

Settings used for 4th and 5th axis programing include:

For the 4th axis: • Setting 34 - 4th Axis Diameter

For the 5th axis: • Setting 79 - 5th-Axis Diameter

For the Axis mapped to the 4th or 5th Axis: • Setting 48 - Mirror Image A-Axis • Setting 80 - Mirror Image B-Axis • Setting 250 - Mirror Image

C-Axis Setting 85 - Maximum Corner Rounding should be set to 0.0500 for 5-axis cutting. Settings lower than 0.0500 move the machine closer to an exact stop and cause uneven motion.

You can also use G187 Pn Ennnn to set the smoothness level in the program to slow the axes down. G187 temporarily overrides Setting 85. Refer to page 393 for more information.

 

 

 

  • Like 1
Link to comment
Share on other sites
14 minutes ago, Colin Gilchrist said:

That all looks pretty good, except the "Max Inverse Time Value", which is way too high.

Try "medium" with Setting 191, which may help "open up the tolerance", if needed.

 

Rotary Axis Command Exceed Precision - That could be from the precision of the rotary axis NC Code "input", but could also be the Inverse Time Feed Values, giving a value that exceeds the Haas Maximum value on the control. 

 

This is great Colin, thanks I'll get hold of this programming manual.  When the customer first reported this problem, the post was running in G94.  Cimco enabled G93 to see if would help and it did help with feeds in some parts of the program but we were still getting the slow five axis motion near B0.  We'll certainly give "medium" a try with setting 191 and we'll get Cimco to limit the max feed in G93 too. 

If I get some feedback from Haas I'll pass it along!

Link to comment
Share on other sites
9 minutes ago, Rich Thomas 4D Engineering said:

This is great Colin, thanks I'll get hold of this programming manual.  When the customer first reported this problem, the post was running in G94.  Cimco enabled G93 to see if would help and it did help with feeds in some parts of the program but we were still getting the slow five axis motion near B0.  We'll certainly give "medium" a try with setting 191 and we'll get Cimco to limit the max feed in G93 too. 

If I get some feedback from Haas I'll pass it along!

If you look at the notes I posted, Haas recommends opening up that 0.025" for Setting 85, to 0.050, for 5-Axis machining. Also, check to be sure both M11 and M13 are commanded before the G93 motion starts. If these aren't explicitly commanded, the machine will auto unlock/lock on each move!

  • Like 1
Link to comment
Share on other sites
Just now, Colin Gilchrist said:

Also, check to be sure both M11 and M13 are commanded before the G93 motion starts. If these aren't explicitly commanded, the machine will auto unlock/lock on each move!

^^^^^This^^^^^

I have seen the issue and it was caused by this right here

Link to comment
Share on other sites
2 minutes ago, Colin Gilchrist said:

If you look at the notes I posted, Haas recommends opening up that 0.025" for Setting 85, to 0.050, for 5-Axis machining. Also, check to be sure both M11 and M13 are commanded before the G93 motion starts. If these aren't explicitly commanded, the machine will auto unlock/lock on each move!

 

Just now, JParis said:

^^^^^This^^^^^

I have seen the issue and it was caused by this right here

Thanks guys 😊 We have already tried opening up Setting 85 to 0.05" but the customer told me that it didn't make a difference to the slow feed sections.

We do have M11 and M13 before the G93 (and the G234 as it happens).  

FYI, For a while we thought the slow feeds were due to large C-axis motions between blocks in the NC code (because there were some large C-axis moves of 50 degrees for example in the program).  Cimco has a Misc Real called Max Angle Movement and we enabled it and set it to 5 degrees... that didn't help.  We then went down to 1 degree and it made the NC program three times larger but still didn't help with the slow feeds near vertical.

 

P.S.  Holy off-topic posts Batman!  I'm so sorry that I've taken this thread so far off-topic by the way - I hate that when I see it myself!

Link to comment
Share on other sites

Just a quick update... Haas USA tell me that there is a bug in an older release of the UMC software that causes slow feeds in 5-axis when TCPC is active, so this is looking like the culprit.  We've also ran the same NC code on another UMC750 now without a problem.  So it seems Mastercam and the post wasn't at fault at all 😊 Thanks for all of your help and advice chaps!

  • Like 3
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

  Only 75 emoji are allowed.

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

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 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

×
×
  • Create New...