What's new
What's new

Accuracy of Brother W1000Xd2

All this M298 business is part of the new Quick Setting function that redoes all the High Accuracy interface. Another feature of Quick Setting is that you can set the machine up with a Default Mode, so all the program you run will have that mode applied. Obviously, their intent is for you to use Standard (M298 L1) in this slot, but you can use whatever you want.
Where exactly can one find the spot for specifying default smoothing setting? One of our machines somehow got set to M298L5 as default and I want to change it.
 
Not that I own a Brother (wish I did) but is that Mode B thing because the control curve fits its own spline or arc through the G01 moves based on L setting tolerance? Pretty cool if so. Would love to just feed my Fanuc big code and not worry about memory size or baud rates/data starvation etc.

The L codes are different "Modes". Rough, Medium Rough, Finishing, etc.

Within the settings of those modes, I have some control over how splines are fitted using Mode B. For example, there are 6 modes, and two of them (Medium Roughing S and Finishing S) are designed for complex contour geometry.

How Fusion picks each mode is up to the post and how creative post makers want to get with their setup.

I use NX, and I skip this entire challenge and just use the Methods architecture. In NX, "Method" sets up all sorts of variables about a tool path - tolerances, machine output (arcs and lines, or G01 lines only), simulation color, etc. My post uses the Methods name to set the mode.
 
Where exactly can one find the spot for specifying default smoothing setting? One of our machines somehow got set to M298L5 as default and I want to change it.
User Parameters/High Accuracy "Quick Settings" screen - the very top is a column row that lets you choose the default option. The area at the top of the screen highlighted in blue.
 

Attachments

  • Screenshot 2024-06-03 at 3.50.09 PM.png
    Screenshot 2024-06-03 at 3.50.09 PM.png
    5.7 MB · Views: 21
It depends on the post. I think the Autodesk Haas post uses stock to leave as the primary driver of selecting from their G187 codes, and that followed onto the Autodesk Brother post, where they just use Finish and Rough (mostly).

3rd Party users have done all sorts of stuff - like using the kind of operation + stock to leave, to using the Smoothing option in the operation to make decisions.

One big thing I see people do is use "Smoothing" in Fusion, which is a NoNo on the Speedio for surfacing. If you are doing surfacing, or continuous curvature corner rounds, or any sort of spline geometry - you want to output G01 moves. Do not try to fit arcs to this geometry, as Mode B will not process them. You have plenty of memory, even in a C00 - just send a pile of code to the machine, it will crunch through it better than if you try those old-school tricks to compact the file.

Greg, can you give me a bit more reference on the spline comment? Is this only for 3D stuff? At least for 2D stuff I've always tried to output arcs since it seems substantially smoother and faster to run on my S700X2 machine?

Re the question on auto smoothing levels. See the link here. This is my slightly tweaked heuristic, but broadly we are using stock to leave as the basic heuristic to decide what mode to use. However, based on Greg's comments above, I might tighten those bounds quite a bit more (so we use roughing modes more often).

I've also started to try and track operations which should always be run in "finishing" mode, eg bores or contours. Otherwise I surprised myself when I did creative things like offsetting a contour and suddenly it's running in full roughing mode. (You can always override it if needed though). I also am starting to push some other ops into a force roughing mode, like facing (keeps the movement smooth). I would be grateful for experts like Greg adding more thoughts on this since these are all heuristics... I could for example force the 3D smoothing moves for some ops?

 
"Set the feed high enough you can check it's not speed limiting on any of the accuracy modes?" I don't understand what you mean since any accuracy mode will slow it down at nearly any speed. I do remember that our machines behave quite differently so we may be running into that again.

No, I'm referring to the max speed "on the straights".

The Brother has about 5 places you need to set the max feed rates. If you ONLY change the user option then it will allow you to feed faster in L0 mode, but you will be speed limited in the high accuracy modes. There are different limits for Mode A vs Mode B modes. I would need to go to the machine to list them all

My point is to setup a simple test contour with sharp corners and a wide corner. Then have the machine transition that, while changing the Lx param each run. Set the feed speed to be the max feed rate you think the machine should run at. Now run your program and if it's not running at that feed rate then there is your problem!! In my case I *thought* I had changed all the limits, but I was stuck at a much slower feed rate whenever certain accuracy modes were enabled, hence why I *thought* L1 was running faster than full roughing L2.

Seriously, it's just a quick contour to run up. Take a large square, put a fillet on a corner, other 3 corners are sharp. I honestly think if you run the machine around that at a high feed, then vary the accuracy modes, you will immediately see how the various L modes interact with the practical path. Just watch the feed rate on the display, it makes it super obvious what must happen! Like if you ask it to make a sharp corner on L0, then watch the screen, you will NOT see the feed speed flicker! So QED it's trying to run the corner at high speed and we can do some maths to figure out how much it must be cutting the corner (or Greg might be able to say that it has other limits?)


I don't have any machine definitions so I will look into that.

Yes! You need these for the home position today and that in turn is used for retract position!! Beware!!

However, it always seemed like a hack to have the buttons on the post page for the rotary axis. Latest upstream autodesk now emits warnings if you use these... My guess is they will remove them completely in the future (and I agree).

Setup the machine def as you want it, (like in your case you have A and B reversed). Much better


Here is the culprit part showing the .02" radius. This is Op2 and it is a bar of 10 parts nested into a fixture held in place with 10-24 screws from the back. Because the parts are nested I need to maintain a tight tolerance on the profile, which then forces me to do the same for the corner radiuses top and bottom. When using L3 the tool barely touched the inside corners and clipped the outsides of the legs. I usually use L1 to finish with for everything but sometimes I have to tighten it up a bit.

I would immediately expect to use L1 on this. My default feed for aluminium would be around 236ipm for chamfering. I mostly use L1 and can't say that I can see visible deviation from perfect?


For reference I am holding .0003" on the width of the legs as they taper from the end to the center so I need some fairly tight tolerances on this part. My other machine is a 2001 Kitamura with a Yasnac control with the optional high speed machining card. It will hold the same or better tolerances as the Brother on L5 but I can not detect it slowing down on a 90 degree .005" cutter path radius until 165 ipm, so it sets the bar pretty high.

Yeah, I think we agree that the machine slows down "excessively" with L5. Theoretically it should be able to change velocity quickly enough to corner faster than it does in L5.

My wild guess is that the feedback loop is used to drive it around the corner, rather than a forward looking predictive motion? So it's overly cautious in order to maintain it's accuracy margin? I wonder if the D00 controls can run faster in L5?

However, as Greg says, you might want to experiment with ensuring you are sending arcs for L5 (did I get that the correct way around?). At least empirically I find that G1 lines are quite slow in L5 mode, arcs are massively faster (click "smoothing" in fusion).

Intuitively it seems to me that in L5 mode, connections between arcs are treated as an exact stop, (not sure about a G1 to arc connection?). So where 2 arcs connect you have the machine slow down as it transitions through the connecting point. I guess you can imagine a gymnast running down a series of tightrope wires. They can really sprint on the straight sections, but where you have two corners come together they need to really slow down to make the corner (no margin for deviating from the wire path on a tightrope, need to corner slowly)? In theory they can also sprint around a corner section of wire, but that doesn't seem implemented in the Brother C00 control and it proceeds quite cautiously around these curved sections?
 
No, I'm referring to the max speed "on the straights".

The Brother has about 5 places you need to set the max feed rates. If you ONLY change the user option then it will allow you to feed faster in L0 mode, but you will be speed limited in the high accuracy modes. There are different limits for Mode A vs Mode B modes. I would need to go to the machine to list them all

My point is to setup a simple test contour with sharp corners and a wide corner. Then have the machine transition that, while changing the Lx param each run. Set the feed speed to be the max feed rate you think the machine should run at. Now run your program and if it's not running at that feed rate then there is your problem!! In my case I *thought* I had changed all the limits, but I was stuck at a much slower feed rate whenever certain accuracy modes were enabled, hence why I *thought* L1 was running faster than full roughing L2.

Seriously, it's just a quick contour to run up. Take a large square, put a fillet on a corner, other 3 corners are sharp. I honestly think if you run the machine around that at a high feed, then vary the accuracy modes, you will immediately see how the various L modes interact with the practical path. Just watch the feed rate on the display, it makes it super obvious what must happen! Like if you ask it to make a sharp corner on L0, then watch the screen, you will NOT see the feed speed flicker! So QED it's trying to run the corner at high speed and we can do some maths to figure out how much it must be cutting the corner (or Greg might be able to say that it has other limits?)




Yes! You need these for the home position today and that in turn is used for retract position!! Beware!!

However, it always seemed like a hack to have the buttons on the post page for the rotary axis. Latest upstream autodesk now emits warnings if you use these... My guess is they will remove them completely in the future (and I agree).

Setup the machine def as you want it, (like in your case you have A and B reversed). Much better




I would immediately expect to use L1 on this. My default feed for aluminium would be around 236ipm for chamfering. I mostly use L1 and can't say that I can see visible deviation from perfect?




Yeah, I think we agree that the machine slows down "excessively" with L5. Theoretically it should be able to change velocity quickly enough to corner faster than it does in L5.

My wild guess is that the feedback loop is used to drive it around the corner, rather than a forward looking predictive motion? So it's overly cautious in order to maintain it's accuracy margin? I wonder if the D00 controls can run faster in L5?

However, as Greg says, you might want to experiment with ensuring you are sending arcs for L5 (did I get that the correct way around?). At least empirically I find that G1 lines are quite slow in L5 mode, arcs are massively faster (click "smoothing" in fusion).

Intuitively it seems to me that in L5 mode, connections between arcs are treated as an exact stop, (not sure about a G1 to arc connection?). So where 2 arcs connect you have the machine slow down as it transitions through the connecting point. I guess you can imagine a gymnast running down a series of tightrope wires. They can really sprint on the straight sections, but where you have two corners come together they need to really slow down to make the corner (no margin for deviating from the wire path on a tightrope, need to corner slowly)? In theory they can also sprint around a corner section of wire, but that doesn't seem implemented in the Brother C00 control and it proceeds quite cautiously around these curved sections?
Since Yamazen changed the max feed I assume it was done where needed but will do the test, it's not like I need to cut metal to do it.

I like the buttons on the post page to disable the rotary when I am not using it so I hope AD doesn't do away with them.

It would be interesting to compare machines on this part, but I can assure you I started with L1 and then tightened it up until I got a satisfactory part, which did not happen until I used L5. I do a couple thousand a year 20 per cycle so if I can save a few seconds I will, and never stop trying. If you stay with the same accuracy level then the chamfers and corner rounders look good and even, even if the profile wonders a few thousandths, .1mms ish. You should try chamfering the profile you finished with L1 using L5 and see how close to perfect L1 is, I know on my machine there is a big difference. My default for chamfering in production is 400-500 ipm with a 1/4" diameter six flute double angle mill. I have played with going faster but on the part I was making the cycle times started to increase

I think the slow down to maintain accuracy is predictive based on slowing the feeds with the override knob on the control. The feeds slow down the same percentage, straights or corners. If it was feedback I would think it wouldn't slow down as much in the corners when overriding the feeds.

I agree the Brother doesn't like short segments. I have had Fusion create .01", .25mm, long lines at the end of longer ones and it made my machine stumble hard even though there was no change in direction. Or where Fusion posted 5 short line segments instead of an arc. Once I replaced the segments with an arc it ran noticeably smoother. In both of these instances I was probably using L1.
 
Great thread. My default Inventor CAM post uses m265, m261. I added M286 for roughing/ not cutting moves >400ipm. Funny I've only used M298 L2 for 3d surfacing. For a roughing mode, the surfaces sure come out nice (maybe not accurate ?). Motion is smooth and fast. I'm not doing mold work/cosmetic finishes. Mostly for clearance or Air/liquid flow. Customers are happy, and I get'em done quick. I could learn a lot from you production guys, but for now, it's " low hanging fruit" 😋
 
Great thread. My default Inventor CAM post uses m265, m261. I added M286 for roughing/ not cutting moves >400ipm. Funny I've only used M298 L2 for 3d surfacing. For a roughing mode, the surfaces sure come out nice (maybe not accurate ?). Motion is smooth and fast. I'm not doing mold work/cosmetic finishes. Mostly for clearance or Air/liquid flow. Customers are happy, and I get'em done quick. I could learn a lot from you production guys, but for now, it's " low hanging fruit" 😋
L4 and L6 is for surfacing, "smoothing".
 
I have more U500s in my region than anywhere else - of course, I'm the Yamaen rep, so I am biased, right? So instead of singing praises, let me just outline the quantifiable facts:

1- Every U500 customer we have in this region (Pacific Northwest), either has already bought another U500, or plans to buy another U500 as soon as the business scale calls for it. We already have substantial fleets of U and M machines established in this area, and those customers plan on continuing to scale out with these machines.

2- About 1/4th of the U500s sold have gone to 5 axis shops with very high end equipment, and were originally purchased for doing roughing or low-tolerance work to free up the expensive spindles. What has actually happened is that customers are finding the U500 is keeping up with the bourgeoisie machines as far as accuracy and surface finish, while reducing cycle times by 30% in many cases. So the machines are not doing roughing - they are doing all the production jobs that can work within the U500 envelope and tool capacity. Every single one of these customers are on U500 #2 or #3 (one is planning on #6-#10).

3- The newer machines are all full 5 axis now (the 4+1 is still built, but we've decided to only stock the full 5). We also have graphical probing from Blum and Renishaw, as well as kinematic setting kits (macros + calibration balls) and CAMPlete is now fully configured for the U500. Esprit, MasterCAM, and NX have also done full post/sim kits for their respective packages at this point. Like any new machine, we had some very minor teething issues at first, mostly everyone figuring out the 5 axis stuff, but everything is very well sorted now. Reliability has been typical Brother - as the guy who gets to count all the warranty claims for the largest overall fleet of U500s, let me look up how many warranty issues the U500s have had in the last 24 month... Zero.

List price is $175k. Even with all the options (1k PSI Through Spindle Coolant, probes, etc), you are under $200k, so within spitting distance of the UMC500SS.

I own an S700. Given that I work at Yamazen, upgrading to a U500 is not exactly in the cards (I'm the sales guy for 4 states, so it isn't like I have a lot of spare time to spend with my machine as it is). If I didn't work here though? I would be a U500 owner, absolutely. It is an incredible machine that performs far above what it has any right to at this price point.
What is the distance from the spindle face to the center line of rotation on the U500? I am going to buy a machine with 5 axis positioning in the future, either a positioning trunnion type or full 5 axis. I believe the 5 axis positioning trunnion that just sits on the table might be better for me as I could use shorter gage length tool holders and ultimately have better rigidity. Most of the parts I make would fit in your hand. As I understand it, most machines in the configuration of the U500 would need longer tool holders to reach a small part oriented 90 degrees. Having full 5 axis would be nice though.

There is a very funny video out there of a guy who bought a 5 axis mazak not knowing he would need longer tool holders to reach the part with the machine he picked. I definitely don't want to end up like that guy.
 
The L codes are different "Modes". Rough, Medium Rough, Finishing, etc.

Within the settings of those modes, I have some control over how splines are fitted using Mode B. For example, there are 6 modes, and two of them (Medium Roughing S and Finishing S) are designed for complex contour geometry.

How Fusion picks each mode is up to the post and how creative post makers want to get with their setup.

I use NX, and I skip this entire challenge and just use the Methods architecture. In NX, "Method" sets up all sorts of variables about a tool path - tolerances, machine output (arcs and lines, or G01 lines only), simulation color, etc. My post uses the Methods name to set the mode.
Hello.

Is there any chance you can explain to me how you set this up in NX. I would like to learn how to do this primarily for the Okuma and the Hi Cut mode. Thank you
 
In no way meaning to detour this thread, but want to throw in a piece of information for anyone that is or might be looking for highest possible feed rate and still fall within tolerance... (on a mass-produced part):

I worked at a large tech company quite a few years back, and some of the components being made were VERY high quantity (aluminum). We brought in Heidenhain with one of these: https://www.heidenhain.com/products/testing-and-inspection-devices/machine-tool-inspection/2 , and learned more about tweaking tool paths and machine settings in a couple of days than we could have learned in... well... maybe not ever. fwiw: this testing was done on a new Robodrill.

Granted, the KGM system is limited to testing 2 axis, so can be used to check either X/Y, X/Z or Y/Z. Essentially, the KGM is connected to a laptop that has the CAD profile of a tool path, and the software overlays the path the machine is *actually* doing over the programmed path (enhanced logarithmically so that deviations are visibly obvious). Seeing a visual display of the machine starting to "cut corners" as the feed rate gets high(er) was only a small part of it. What surprised us a lot (at very high feed rates) was seeing how long it took the machine to "track" dead straight again after going around a corner (whether radius or spline) and then back to a straight-line move. We were seeing something akin to a decreasing sine-wave movement as if the machine was "hunting" for where it needed to be -- at very high feed rates, sometimes as many as 5 or 6 plus/minus overshoots until that axis settled into position.
And of course, adding/subtracting mass to the table showed right up in the "true" tool path vs. programmed.

Did we definitively nail down all the fine tuning in the control to make one high volume part better/faster? I'd say that the balance between speed and accuracy is what we found.

More importantly though, the largest benefit of doing that testing was having all the engineers, designers, and machinists clearly see and understand how the machine moved with changes to CAD, feed rate or control tuning.

fwiw...
PM
 
And of course, adding/subtracting mass to the table showed right up in the "true" tool path vs. programmed.

I believe I saw some of the reports from this testing; the impact of table weight was a little shocking. Not just a noticable difference, but a massive difference.

Of course, a KGM system is not the kinda item you can just run down to Fastnell and pick up. Does anyone know roughly what one of those bad boys costs?
 
Hello.

Is there any chance you can explain to me how you set this up in NX. I would like to learn how to do this primarily for the Okuma and the Hi Cut mode. Thank you

Fire up post builder.
Insert a block with a little switch logic in it using the Method name to select each mode.

Bonus points if you build a fresh install of NX and forget the naming scheme you used to drive all this, and you spend about 3 days machining everything in L1 (Standard) because you forgot that you named your Rough methods "Roughing" and your finishing stuff "Fin". Consider a more robust approach, but never get around to implementing it.

"A temporary solution today is downpayment on a headache tomorrow!"
 
This has been a great thread. Thanks for all the info everyone.

We are continuing to look at the brother u500 and notice that the trunnion has capacity of only 200lbs. That seems a little bit light.

@gkoenig can you get the u500 with a larger capacity trunnion to hold more than 200Lbs?
 
This has been a great thread. Thanks for all the info everyone.

We are continuing to look at the brother u500 and notice that the trunnion has capacity of only 200lbs. That seems a little bit light.

@gkoenig can you get the u500 with a larger capacity trunnion to hold more than 200Lbs?

Nope. The weight is derived from the rotary axes that Brother uses - they make no bones about the U500 basically being two of their T200Ad tables slapped together. They have like 5,000 of these in service globally; probably why the U500 has been so successful out of the box is that Brother didn't try to reinvent anything, just derived it from well engineered parts with lots of history behind them. If you know what you are doing, parts bin engineering is a very smart way to build machine tools.

Having said that, I have customers doing pretty large aluminum parts on them with big fixture plates, a giant Schunk KSP160 vise, beefy steel jaws and flipping a 3"x13"x4" chunk of aluminum around like it is nothing.
 
@gkoenig are you able to turn with the U500? I see on the M200 and M300 they can turn but can the U500 also turn?

For turning, is it possible to upgrade to a Capto spindle or do they still use BT30 for spindle? Only reason I ask is because drive keys are the same size on BT30 so the tool can go in spindle either way( which may cause issue for turning applications) and there is slop in between drive dog and drive slot which may affect positioning of turning tool. Just wondering if they use capto instead for greater rigidity and/or positional accuracy?
 
Also, do you think Brother will ever enter the lathe market or get back into the wire EDM market? I wonder why they stopped making EDM machines?
 
@gkoenig are you able to turn with the U500? I see on the M200 and M300 they can turn but can the U500 also turn?

For turning, is it possible to upgrade to a Capto spindle or do they still use BT30 for spindle? Only reason I ask is because drive keys are the same size on BT30 so the tool can go in spindle either way( which may cause issue for turning applications) and there is slop in between drive dog and drive slot which may affect positioning of turning tool. Just wondering if they use capto instead for greater rigidity and/or positional accuracy?

No turning on the U500 - it is designed to handle larger parts where more rigidity is required and both A and C are roller drive (the zero backlash system we're discussing in another thread). On the M series machines, the C axis is direct drive, which is how it gets the turning capability.

And Brother is 100% BT30/Big + BT30. They offer zero other spindle options and we have no indication that is in the cards anytime soon. They did offer HSK40 back in the day, but it was not popular. I actually have a customer here with a couple of HSK40 Brothers - I can tell you that BBT30 is more rigid, has much wider availability, and is a generally more reliable system. I can see arguments for the 27k machines being HSK, but those are very rare - the vast majority of everything we sell is the 16k spindle because is really is a remarkable all-around performer.

On the M series machines, Brother uses a set of pins behind the spindle that engage a flange on the tool holder for turning. Yukiwa, NT, and Big Daishowa make 1" stick tool and boring bar holders to the Brother spec with the flange. Tungaloy and Sandvik both make Brother BT30 Turning to Capto C4 holders so you can use that whole world of tooling.

As far as upcoming machines, they literally tell us nothing.
 
I have more U500s in my region than anywhere else - of course, I'm the Yamaen rep, so I am biased, right? So instead of singing praises, let me just outline the quantifiable facts:

1- Every U500 customer we have in this region (Pacific Northwest), either has already bought another U500, or plans to buy another U500 as soon as the business scale calls for it. We already have substantial fleets of U and M machines established in this area, and those customers plan on continuing to scale out with these machines.

2- About 1/4th of the U500s sold have gone to 5 axis shops with very high end equipment, and were originally purchased for doing roughing or low-tolerance work to free up the expensive spindles. What has actually happened is that customers are finding the U500 is keeping up with the bourgeoisie machines as far as accuracy and surface finish, while reducing cycle times by 30% in many cases. So the machines are not doing roughing - they are doing all the production jobs that can work within the U500 envelope and tool capacity. Every single one of these customers are on U500 #2 or #3 (one is planning on #6-#10).

3- The newer machines are all full 5 axis now (the 4+1 is still built, but we've decided to only stock the full 5). We also have graphical probing from Blum and Renishaw, as well as kinematic setting kits (macros + calibration balls) and CAMPlete is now fully configured for the U500. Esprit, MasterCAM, and NX have also done full post/sim kits for their respective packages at this point. Like any new machine, we had some very minor teething issues at first, mostly everyone figuring out the 5 axis stuff, but everything is very well sorted now. Reliability has been typical Brother - as the guy who gets to count all the warranty claims for the largest overall fleet of U500s, let me look up how many warranty issues the U500s have had in the last 24 month... Zero.

List price is $175k. Even with all the options (1k PSI Through Spindle Coolant, probes, etc), you are under $200k, so within spitting distance of the UMC500SS.

I own an S700. Given that I work at Yamazen, upgrading to a U500 is not exactly in the cards (I'm the sales guy for 4 states, so it isn't like I have a lot of spare time to spend with my machine as it is). If I didn't work here though? I would be a U500 owner, absolutely. It is an incredible machine that performs far above what it has any right to at this price point.
Hi @gkoenig , could you send me a PM please? I'm looking at bringing in a U500 into our shop. My local Yamazen office has been fantastic with the help so far, but it sounds like you might be able to help with a couple extra questions I have. I'm a long time reader, first time posting here, so it looks like I'm not allowed to send out PMs?

Thank you
 








 
Back
Top