Blocks Per Second limit

[brandon_gunderson]

Recently I noticed an issue with my Haas VF2 Surface finish. I was getting gouges all over the place.


Lots of back and forth and a tech coming out and I get an email saying the issue is with how many blocks per second is being output and that I should limit my blocks per second within fusion. Is there a way to do this? I know there are settings for blocks per second within machine parameters but I have found little to no information on it. I'm honestly not sure changing the machine parameters even does anything within fusion.

Any input would be much appreciated.

Thanks.

[nick_p3dcreations]

I would take a look at your smoothing and tolerance settings. I've been able to achieve great finishes on surfacing and fantastic performance on HSM toolpaths, even with old machines. (Speaking of, what year is your VF2 and does it have High Speed Machining enabled?)

Here's a good write-up on it: https://www.autodesk.com/products/fusion-360/blog/best-settings-smoothing-tolerance/

And a video: https://www.youtube.com/watch?v=vt7rVVRiiKk

I did also notice that there's a "Maximum Block Processing Speed" field in the machine configuration menu, but I don't know if it does anything yet. 

[Collin_Korver]

That blocks per second is only for reference, it in no way changes anything. 

Like what @nick_p3dcreations said you have to play with your smoothing settings. When I notice gouges, I will start dropping the tolerance<1.0e-4 and upping the smoothing to max [tolerance*9.99] . Generation time exponentially increases but usually that's better than gouges. I will also avoid 3D tool paths that involve changes in 3 axes (basically sticking to 3d contour/parallel) as these work best for creating the cleanest point to point arcs for smallest file size and largest arcs.  I have also noticed the steep and shallow tool path creates many more gouges than any of the "comprised" toolpaths which is quite unfortunate.

[brandon_gunderson]

I appreciate the help but this is not a toolpath issue. I've thrown the tolerances out of acceptable ranges and that did not fix the problem and neither does smoothing.

I have a minimill and a VF2 SS. The minimill runs the code perfectly, the VF2SS does not. 
I have HSM enabled on both machines. I've taken the tool out of one machine and put it in the other. Everything is the same besides the machines physically, same options, same parameters, same program, same tools. I have done tons of testing on the machine to fix the problem and so has the tech. Haas HQ themselves said the issue is too many lines of code to quickly in the machine since the VF2SS has a 12 pitch screw and the minimill has an 8 pitch. They said limiting the blocks per second will fix the issue.

[Collin_Korver]

On a Haas, to limit block lookahead is G103 P[number of blocks to limit].

So to limit the Block look ahead to 15 blocks is

G103P15;

Then to cancel lookahead limit is just G103.

[Collin_Korver]

Something else you can try is entering G187P3 infront of the finishing pass. This tells the control to prioritize accuracy over speed. 

Then at the end of the section insert G187 to turn that off.

here is what the manual says

G187 Setting the Smoothness Level (Group 00)
G-187 is an accuracy command that can set and control both the smoothness and max corner rounding value when cutting a part. The format for using G187 is G187 Pn Ennnn.
P Controls the smoothness level, P1(rough), P2(medium), or P3(finish).
E Sets the max corner rounding value, temporarily overriding Setting 85.
Setting 191 sets the default smoothness to the user specified “rough,” “medium,” or “finish” when G187 is not active. The “medium” setting is the factory default setting. NOTE: Changing setting 191 to “Finish” will take longer to machine a part. Use this setting only when needed for the best finish.
G187 Pm Ennnn sets both the smoothness and max corner rounding value.
G187 Pm sets the smoothness but leaves max corner rounding value at its current value. G187 Ennnn sets the max corner rounding but leaves smoothness at its current value. G187 by itself cancels the E value and sets smoothness to the default smoothness specified by Setting 191. G187 will be cancelled whenever “Reset” is pressed, M30 or M02 is executed, the end of program is reached, or E-stop is pressed.

[brandon_gunderson]

I'll have to try the G103 command.

I've already messed around with G187 and parameter 191 and tried all of that. Me and the tech went over a lot of **** both mechanically and in the control. I mean we went through everything. They seem convinced it's to do with how many blocks per second the program has.

[Collin_Korver · Accepted solution]

Limiting blocks per second is per the control not the program. So G103 is what you will want to try. If that does any good I would be shocked

[brandon_gunderson]

Yeah, I figured.

I don't see how a line of code could magically do what the control could not. I was really hoping there would magically be some temporary fix but it doesn't appear there is one.

All in all I'm pretty disappointed in HAAS. I've had really good results with my machine for years. We ran a ballbar on it and it's accurate to tenths even at 100ipm and has no problem repeating locations. It's a lighter weight machine but it's a hell of a lot cheaper than others and since I cut 90% aluminum it doesn't really matter to me. They are really standing hard on this being anything but their problem and it's unfortunate. to say the least.

I really dont understand if their control has issues with over 1000 blocks per minute why the control itself doesn't have a limiter. We have an old acroloc that we drip feed programs off of and if it can't read the code as fast as programmed it just slows itself down. I don't see why this should be any different.

[Collin_Korver]

My Vf2SS W/HSM greatly slows down depending if I have G187 P3 vs G187 P1 active, which is limiting the blocks per second (it actually limits accelerations). I dont mean to patronize so there's my disclaimer but blocks per min isnt really a good description of what is going on TBH. What is most important is the difference in time between blocks, the controller's look ahead, the feedrate, and the machines linear acceleration.

Lets say you are traveling at 100 ipm. If you have 60 blocks that each travel 1 inch your effective blocks/sec is going to be 1.66.  It is going to be smooth. If you have 60 blocks that each travel .002" at 100IPM, the effective blocks/sec is about 833. (100IPM=1.66IPS | .002in/1.66IPS =  .0012 sec/block or 833 blocks/sec).  As you can see, it is pretty easy to max out 1000 blocks/second. Keep in mind this isn't taking into account processor delays, changes in acceleration, etc. Look ahead effects how the feed accelerates from point to point. With 0 look ahead it becomes choppy because it is accelerating and decelerating for every block. With HSM it can read 60 blocks ahead and smooth its acceleration between points. In the example above, the machine only has .072 seconds to make  accelerations calculations. If it cant make all the calculations in time, it becomes choppy.

IMO Haas' look ahead is less than satisfactory, so I really work on making sure my program is as smooth as it can be. So like I said earlier to get the smoothest and most accurate tool path one needs to lower your tolerance and max out the smoothing. Smoothing takes a bunch of points does some math, and generates a 2D curve that best incorporates all of the points. BUT lets say your toolpath truly is a 3d tool path moving in xyz. Smoothing to my knowledge only works in 2D arcs, so if you have a true 3d tool path smoothing doesnt do much. This can result in very dense/ splochy tool paths. The tool will be traveling along happly and then suddenly it runs into 100 points that are only .002 inches apart. The machine will max out its look ahead, slow down to make sure it hits all the points within the defined tolerance (bc of accuracy settings), but his slow down can cause surface imperfections/ potential gouges.

I attached Steep and shallow and Parallel tool paths with 'show points' activated as examples. Steep and shallow was forced to just parallel and all the parameters were essentially the same. Tolerance was set to 2e-5 and smoothing for parallel operation was [tolerance*9.99]. Steep and shallow doesnt have the same kind of smoothing, and it shows.

 You can see the "standard" parallel tool path would be much more controler friendly.