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 vs Makino part 2


Bob W.
 Share

Recommended Posts

i did not even evoke g187 (E.xxx on older machines). as far as i'm aware the G187 really is a programmable override to the global setting 85 "max corner rounding. correct me if i'm wrong.

roughing to within .005 is pretty impressive. just outlines how much Mastercam has improved. i would have never thought we could do this in the Pre-X days. I've never trusted cutter deflection that much, so i usually leave .020 to .030 even when confident of the setup.

are you really finishing faster at .005 vs .03? sometimes if a large tool leaves stock in corners, i will do a quik Rest-rough in the corners with the finish tool to the same .02-.03 rough stock, then go for finishing. as long as i'm carefull to be climb cutting it works well for, oh, say a .250ball sticking out 2-3inches.

Link to comment
Share on other sites
Maybe my Haas is just a lemon?

well the 8K on new spindle drive parts woulda royally p'd me off.

someone in this thread mentioned ball screw pitch differences between Haas models; the VM series having the finest pitch. this and that thick table would seem to conspire for slow accelerations that iv'e noticed on that model.

it would be interesting for someone with a modern SS haas to run your code to see the difference Haas to Haas.

 

love the idea of the ring gauge to determine thermal growth. would it make sense to set it about the same distance from the part and the part roughly in the center of travel on both macines?

Link to comment
Share on other sites

I watched your vids mkd. Do you get good results with your corner rounding set to .020"? That seems like a lot to me. But then again our machines do slow down in the corners. Especially the older VF3's.

 

I will be interested to see this thermal growth comparison Bob. I have setups I do that span the entire table in my VF2. I have blends on some parts that have to be done with a flat endmill cutting the same surface from two sides of the part. These blends always remain very nice for me. So if our VF2 was moving around throughout the day I would see it. And I don't. I hold tolerances in the .0002-.0005" all the time which are verified my a newer Mitutoyo CMM. So I am very curious to see how your test does.

Link to comment
Share on other sites

I was thinking for my next video I would run a mold on both machines. What I had in mind was a 12" x 12" aluminum mold. I plan to rough, semi finish, and finish. Before running the mold I would put a ring gage on the back left corner of the table and set a work offset to it. I would also set a reference tool in the spindle. After the mold is complete I would reset the work offset on the ring gage and reset the tool in the spindle noting the results (dimension changes). I will also note the cycle times. All roughing will be done in roughing mode (G187P1 for Haas, M251 for Makino) and all finishing will be done in finishing mode (G187 P3 for Haas, M250 for Makino). This would give a good indication of table drift in X and Y, and spindle growth in Z. Before I run this, are there any suggestions of what people would like to see? Any things I might be doing to make this unfair?

 

This would be a great test. I would love to see your results using your suggested parameters.

 

 

roughing to within .005 is pretty impressive. just outlines how much Mastercam has improved. i would have never thought we could do this in the Pre-X days. I've never trusted cutter deflection that much, so i usually leave .020 to .030 even when confident of the setup.

 

 

Roughing to even closer than .005" is easily attainable on a Makino. This has nothing to do with Mastercam. It has everything to do with Makino's algorithms for accel/decel control, 1000 block look-ahead, Super Geometric Intelligence. If the part is programmed properly, all tool deflection will be away from the part anyways. I have been running Makino's for 9 years and I cannot think of a single instance of a gouge, clipped corner or where something didn't clean up from roughing.

 

As for the HAAS, what I find laughable, is that the setting 85 you mentioned earlier, is set at .050 from the factory. I took HAAS service/applications to task about this and we ran a sample part, basically a pyramid where each z-level represented a different value for setting 85. The performance and feedrate difference between the levels was ridiculous. Sure, if you allow the machine to clip corners, it will maintain feedrate, however, when you set setting 85 to a value that is more realistic for real-world machining, the machine just dies on complicated geometry. The Makino doesn't really care. It just holds tolerance, Period.

Link to comment
Share on other sites
Roughing to even closer than .005" is easily attainable on a Makino. This has nothing to do with Mastercam. It haseverything to do with Makino's algorithms for accel/decel contro............. If the part is programmed properly, all tool deflection will be away from the part anyways.......

back in the MC 6,7,8 and 9 days achieving this was not nearly as streamlined as it is in the post X3 days, particularly for a newbie, particularly for the HS toolpaths. for a newbie to figure out how to create the proper boundaries to get the desired results used to be a daunting. most CNC programs in the 1990s and beyond just hammered away at the material (blanket statement i'm going to get crucified for, haha).

today you pick a solid, fudge a boundary and let Mastercam crunch and get butter smooth motion.

everything to do with Mastercam.

agree with everything else you said +1

Link to comment
Share on other sites

i did not even evoke g187 (E.xxx on older machines). as far as i'm aware the G187 really is a programmable override to the global setting 85 "max corner rounding. correct me if i'm wrong.

roughing to within .005 is pretty impressive. just outlines how much Mastercam has improved. i would have never thought we could do this in the Pre-X days. I've never trusted cutter deflection that much, so i usually leave .020 to .030 even when confident of the setup.

are you really finishing faster at .005 vs .03? sometimes if a large tool leaves stock in corners, i will do a quik Rest-rough in the corners with the finish tool to the same .02-.03 rough stock, then go for finishing. as long as i'm carefull to be climb cutting it works well for, oh, say a .250ball sticking out 2-3inches.

 

I'm usually finishing with tools from .125" down to .030" in diameter so I put a lot of time into the roughing. If I leave .020"-.030" of stock I can't finish with the small tools without adding an intermediate step. Roughing to .005" works great as long as the cutter is always climbing.

Link to comment
Share on other sites

I watched your vids mkd. Do you get good results with your corner rounding set to .020"? That seems like a lot to me. But then again our machines do slow down in the corners. Especially the older VF3's.

 

I will be interested to see this thermal growth comparison Bob. I have setups I do that span the entire table in my VF2. I have blends on some parts that have to be done with a flat endmill cutting the same surface from two sides of the part. These blends always remain very nice for me. So if our VF2 was moving around throughout the day I would see it. And I don't. I hold tolerances in the .0002-.0005" all the time which are verified my a newer Mitutoyo CMM. So I am very curious to see how your test does.

 

My VF2 was pretty solid regarding thermal growth as well, and overall it was a much better machine than the VM3. I would have preferred to keep it and unload the VM3 a few years back but I just needed the travels. In my experience the VM3 is much less stable than the VF2 when it comes to long term accuracy. I was much happier with the performance on the VF2 for sure. Faster, more accurate, and more stable.

Link to comment
Share on other sites

Bob,

Did Haas give youe some parameters to change for thermal growth in the VM-3. IT is supposed to hold tighter then the VF-3. I have a 2010 VM=3

I did have the change the SL-10 Parameters for "X". It calmed it down. I only have to adjust for about .001" in "X" when the machine gets warmed up.

 

MachineGuy

Link to comment
Share on other sites

Bob,

Did Haas give youe some parameters to change for thermal growth in the VM-3. IT is supposed to hold tighter then the VF-3. I have a 2010 VM=3

I did have the change the SL-10 Parameters for "X". It calmed it down. I only have to adjust for about .001" in "X" when the machine gets warmed up.

 

MachineGuy

 

 

They did. I actually spent about three weeks tuning the thermal growth parameters using the probe and a program that looped and collected data. I got it about as close as I could but it is still not perfect. Their thermal comp algorithms leave a lot to be desired. I adjusted for X, Y, and spindle growth. The Z couldn't be dialed in and after the factory service tech spent a week trying they agreed to add a scale. Basically, the longer the machine is running the greater the thermal comp error. For short programs that are constantly starting and stopping it isn't that bad, but for a mold that might run for 10 hours it is terrible. Funny they would have this issue on a 'mold machine'...

Link to comment
Share on other sites
Their thermal comp algorithms leave a lot to be desired. I adjusted for X, Y, and spindle growth. The Z couldn't be dialed in and after the factory service tech spent a week trying they agreed to add a scale. Basically, the longer the machine is running the greater the thermal comp error. For short programs that are constantly starting and stopping it isn't that bad, but for a mold that might run for 10 hours it is terrible. Funny they would have this issue on a 'mold machine'...

 

Yep. It's complicated enough engineering to properly apply thermal growth algorithms to a machine that has cooled ballscrews and temperature sensors all over the place. Now take that same level of complexity - and remove the core cooled ballscrews and actual temperature feedback from air, column, base, spindle, etc - and you've got a whole lot-a nothing.

Link to comment
Share on other sites
are you really finishing faster at .005 vs .03?

 

I would answer "yes" if you are on a Haas. .010" even in aluminum and you can have measurable deflection at even remotely acceptable feedrates.

 

 

I was thinking for my next video I would run a mold on both machines. What I had in mind was a 12" x 12" aluminum mold. I plan to rough, semi finish, and finish. Before running the mold I would put a ring gage on the back left corner of the table and set a work offset to it. I would also set a reference tool in the spindle. After the mold is complete I would reset the work offset on the ring gage and reset the tool in the spindle noting the results (dimension changes). I will also note the cycle times. All roughing will be done in roughing mode (G187P1 for Haas, M251 for Makino) and all finishing will be done in finishing mode (G187 P3 for Haas, M250 for Makino). This would give a good indication of table drift in X and Y, and spindle growth in Z. Before I run this, are there any suggestions of what people would like to see? Any things I might be doing to make this unfair?

 

Just for the record, I add G187 all over the place to help speed things up or make things more precise depending on the toolpath. You have to if you want to maximize those two things on a haas. Otherwise, like mentioned, you are completely stalling the machine as it tries to hit its targets or you are completely cutting through your targets

 

 

 

Moving along pretty good. Is that in G187P1 (roughing) mode? Maybe my Haas is just a lemon?

I assume you are using G187 P... and E...? It is a little strange but I find I need to mess with both a bunch to get to where I need to be.

 

As far as it being a lemon...? No, they all work that way.

 

 

well the 8K on new spindle drive parts woulda royally p'd me off.

someone in this thread mentioned ball screw pitch differences between Haas models; the VM series having the finest pitch. this and that thick table would seem to conspire for slow accelerations that iv'e noticed on that model.

it would be interesting for someone with a modern SS haas to run your code to see the difference Haas to Haas.

 

love the idea of the ring gauge to determine thermal growth. would it make sense to set it about the same distance from the part and the part roughly in the center of travel on both macines?

 

As far as my offer goes to run this on a late model VF3SS it still stands.

 

 

 

 

This would be a great test. I would love to see your results using your suggested parameters.

 

 

 

Roughing to even closer than .005" is easily attainable on a Makino. This has nothing to do with Mastercam. It has everything to do with Makino's algorithms for accel/decel control, 1000 block look-ahead, Super Geometric Intelligence. If the part is programmed properly, all tool deflection will be away from the part anyways. I have been running Makino's for 9 years and I cannot think of a single instance of a gouge, clipped corner or where something didn't clean up from roughing.

 

As for the HAAS, what I find laughable, is that the setting 85 you mentioned earlier, is set at .050 from the factory. I took HAAS service/applications to task about this and we ran a sample part, basically a pyramid where each z-level represented a different value for setting 85. The performance and feedrate difference between the levels was ridiculous. Sure, if you allow the machine to clip corners, it will maintain feedrate, however, when you set setting 85 to a value that is more realistic for real-world machining, the machine just dies on complicated geometry. The Makino doesn't really care. It just holds tolerance, Period.

 

I leave the default at P3 and .0001" for G187 and change it in the program. Since I do a ton of prototyping, the last thing I want is to have the machine cutting any corners that I may not think it will cut. This way, I am in control of how loose the thing runs.

 

 

 

My VF2 was pretty solid regarding thermal growth as well, and overall it was a much better machine than the VM3. I would have preferred to keep it and unload the VM3 a few years back but I just needed the travels. In my experience the VM3 is much less stable than the VF2 when it comes to long term accuracy. I was much happier with the performance on the VF2 for sure. Faster, more accurate, and more stable.

 

The VM3 is a noodle of a machine if you base it on footing size for travels, weight of machine for travels, overhang of the spindle based on the Y travel...etc. Nevertheless...what you say is pretty eye opening comparing it to the VF2. I guess simply being more compact allows the VF2 to shine over the VM3.

 

 

 

Here are some pictures. They show the width of the feet at the rear of the machines. They are both from my 40 X 20" machines. One is a Haas. The other one isn't. :laughing:

post-8694-0-18939900-1358791391_thumb.jpg

post-8694-0-10949500-1358791406_thumb.jpg

Link to comment
Share on other sites

"Just for the record, I add G187 all over the place to help speed things up or make things more precise depending on the toolpath. You have to if you want to maximize those two things on a haas. Otherwise, like mentioned, you are completely stalling the machine as it tries to hit its targets or you are completely cutting through your targets"

 

I never have used that function and both my roughing and finishing come out fine. No stuttering what so ever. If I need accuracy, I'll make a pick up and set the tool length offset prior to running that tool (to account for thermal growth) and use wear. Piece work, not production.

 

Tool deflection when finishing: If I leave .01 or .02 stock on Aluminum, I never see deflection. Of course, I'm not looking for .0002.

 

Mayby we got lucky here, but I'm not seeing alot of the issues reported with the Haas's.

Link to comment
Share on other sites

I never have used that function and both my roughing and finishing come out fine. No stuttering what so ever. If I need accuracy, I'll make a pick up and set the tool length offset prior to running that tool (to account for thermal growth) and use wear. Piece work, not production.

 

 

You should try the G187 sometime. Your machine will run up to 50% faster depending on the feed rates but you do need to make sure and leave adequate stock. If you are leaving .020" you should be okay if the feed rates aren't above 200-250 ipm. Here are the g-codes:

 

G187 P1 (roughing)

G187 P2 (standard - default)

G187 P3 (finishing)

 

G187 at the end of the toolpath cancels the mode and returns it to default. If you are roughing large parts it will save a ton of time.

Link to comment
Share on other sites
  • 1 month later...

Haven't had any time to make more videos but I did make a mold recently on the PS95 and it did very well. This aluminum mold ran for 18 hours and when the machine stopped I probed the X,Y reference point into another work offset and the shift was .0003" in X and .0003" in Y. Needless to say I was very pleased. The finish was also nice enough that on a wallet sized area and 600 grit wet/dry sandpaper it took less than 30 seconds to remove all tool marks. This was machined with a 1/8" ball mill and .005" stepover. Just throwing information out there for anyone that might find it useful.

Link to comment
Share on other sites

HAAS / HURCOS and MILLTRONIC'S

I had to leave stock and then see what It did compared to what I told it to do, and then tweak the program and sometimes the Geo.

I call it "50 trips to the Comparator" it's actually 2 trips. ( To hold +/- .0005)

It works.

Makino / Micron's : dead nuts no matter what, insane, your never chasing your tail.

 

$ Triple the price though $

Link to comment
Share on other sites

$ Triple the price though $

 

This is a budget Makino but IMHO it gives far more than budget results. Now my A51 is a hell of a lot faster and it was triple the price, but this PS95 only cost 50% more than I paid for my Haas VM3 "mold machine" 5 years ago. "Mold machine" LOL!, wait, I paid $100k for that :ouch:

Link to comment
Share on other sites

I should also add that while the PS95 puts down a fantastic finish, the A51 puts down a finish that literally makes me laugh. It ran for 60 hours on a 300Mb program and it really didn't even need to be touched when it was done.

 

It really blows my mind how accurately these can machine parts. I'm talking ANY high end machine, whether it is Makino, Matsuura, Mori, etc... Unbelievable quality and very fun to work with.

Link to comment
Share on other sites

I took delivery of our second PS95 on Friday. There are a number of improvements from our first one that just tuned 2 years old last week. It will be interesting to see the differences once it is set up later this week. Supposedly, Makino made some software improvements that make it 30% faster for 3D machining. Not to say it was slow in the first place. They are going to upgrade the software in our first PS95 too. We also have a new Mikron HSM 700 scheduled for delivery at the end of April.

Link to comment
Share on other sites

not to discount the supreme awesomeness of high end technology, i was just wondering about quantities and what they call a cash-cow in business.

 

I recently read Haas has shipped out their 125,000th machine. the span between that and the 100K mark comes out to about 600-800 machines a month :clap::blink: :blink:

i am having a hard time even wrapping my head around one assembly line here in Oxnard making those kind of numbers.

anyone know how many machines Makino makes in a month? curious.

 

i wish i had the opportunity to compare different machines head to head like Bob. cool stuff indeed!

Link to comment
Share on other sites

oh and WOW 300mb program. jeeze that's a biggie.

largest one i ever did was 22Mb on a 6' x 4' x 4' form tool. on a 5axis no less.

 

Yeah, it was great! It ran 24 hours a day for a few days. I headed out and went for long bike rides :-) It was all the same tool as well...

Link to comment
Share on other sites

not to discount the supreme awesomeness of high end technology, i was just wondering about quantities and what they call a cash-cow in business.

 

I recently read Haas has shipped out their 125,000th machine. the span between that and the 100K mark comes out to about 600-800 machines a month :clap::blink: :blink:

i am having a hard time even wrapping my head around one assembly line here in Oxnard making those kind of numbers.

anyone know how many machines Makino makes in a month? curious.

 

i wish i had the opportunity to compare different machines head to head like Bob. cool stuff indeed!

I know Hitachi used to have machine serial numbers that went (for example) 7, 12, 15, 18, 25 blah blah....It gave a bit of a 'feel good' factor that you didn't have machine number 3 off the production line (but in reality you may have :lol:)

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...