how to make hsm really hsm?

[mig]

Anybody using HS hybrid tool path?

Machine in fact moving very slow because path divided on very small movements even if it not necessary at the moment .

I trying to play with smoothing option but not help much .

Anyone have an idea how to dress this issue ?

Control is Fanuc 18i (HPCC is on )

Thank you in advance

[Guest CNC Apps Guy 1]

How many block look ahead?

[mig]

How many block look ahead?

600 i guess

It not always slow.

[RandleXX]

HSM toolpaths produces a lot of arcs. If your controller is set to slow down in the corners, the overall feed may appear to be a lot slower. Most controllers with this option have the ability to adjust the arc feedrates (contour control) with an G Code setting. You may need to find the perfect balance of contour control and speed.

 

If I remember correctly Fanuc is somthing like G05 P1000

P being the ajustable feed setting. I would look in your machine tool manual to find the exact code needed for your control.

[Chris Rizzo]

filter on in the toolpath?

[Guest CNC Apps Guy 1]

If I remember correctly Fanuc is somthing like G05 P1000

P being the ajustable feed setting.

 

G5P10000 is HPCC on, G5P0 is off. There is no seting for P, it's 10000 or 0. SOmetimes on AI-NANO II, you have a G5.1Q1 Rx., with the "x" being a value between 0 and 10. 0 being I prefer speed over accuracy and 10 being accuracy is the #1 consideration with ACC/DEC being handles accordingly.

[RandleXX]

G5P10000 is HPCC on, G5P0 is off. There is no seting for P, it's 10000 or 0. SOmetimes on AI-NANO II, you have a G5.1Q1 Rx., with the "x" being a value between 0 and 10. 0 being I prefer speed over accuracy and 10 being accuracy is the #1 consideration with ACC/DEC being handles accordingly.

 

 

^^^

Yep, that's the one.. G05.1 Q R

[mig]

HSM toolpaths produces a lot of arcs. If your controller is set to slow down in the corners, the overall feed may appear to be a lot slower. Most controllers with this option have the ability to adjust the arc feedrates (contour control) with an M Code setting. You may need to find the perfect balance of contour control and speed.

 

If I remember correctly Fanuc is somthing like G05 P1000

P being the ajustable feed setting. I would look in your machine tool manual to find the exact code needed for your control.

Yeas my HPCC control is ON but on rough mode.

I still thinking how to set filtering/smoothing options in right balance to reduce number of blocks

[Joe788]

Mig, it just takes experimentation. Smooth, accurate, fast 3D machining is like black magic. Some machines work better with PILES of code. Some machines work better with less code and more arcs filtered in.

 

You just need to experiment. I'd try NO arc filter, and turn the tolerance down to .0001 or less.

[MotorCityMinion]

"G5P10000 is HPCC on, G5P0 is off. There is no seting for P, it's 10000 or 0."

 

That's how our Makino S56 is set up. The manuals also speak of M codes that give you options for high accuracy, high speed and something in between, although I have not messed with those yet. There's yet another setting on the custom page for high accuracy, I turn it on, start the prog and it shuts off. Obviously we don't have a handle on that yet. As far as the code output, I've found that if I set the filter to on, with a tolerance of .00005 to .0001, I get very few arcs in the code, but the machine actually hits the programmed feed, if I set it up with a looser tolerance and mostly arcs, it can stumble some.

 

I'm thinking the shape of the surfaces and the tool size plays in here as well. Ditto what Joe says.

 

Here's a link to a video on filter settings and smoothing that discuss when and where and how to apply them. This may help some. The video is called HSTWebinar.

 

http://www.emasterca...=1

[SKIR68]

There is also a c-hook to change your point to point code to lines and arcs.

[CarbonCAD]

We have a new V56I Makino and we are working out the bugs. When trying to cut a 6" pocket it was .0005"/.0006" out of round, but the other dimensions were fine. The part must be accurate within .0001". This was with breaking the circle geometry into 20,000 straight segments. Line segments is what was recommended by our reseller. Prior to that we tried I's and J's with poor results. With all the options available it is hard to have a place to start. MotorCityMinion maybe you have found some answers since posting about your S56, or does anyone else have suggestions?

[Joe788]

Ouch! .0005-.0006?? Unless you're talking about millimeters, I'd be on the phone with Makino, asking when my new machine is showing up.

[GoetzInd]

Have you tried programming the M252 ultra accuracy mode?

 

Mike

[Cannon]

G5P10000 is HPCC on, G5P0 is off. There is no seting for P, it's 10000 or 0. SOmetimes on AI-NANO II, you have a G5.1Q1 Rx., with the "x" being a value between 0 and 10. 0 being I prefer speed over accuracy and 10 being accuracy is the #1 consideration with ACC/DEC being handles accordingly.

 

This works also in HPCC, G05 P10000 R1.-R10.

[Redfire427]

We have a new V56I Makino and we are working out the bugs. When trying to cut a 6" pocket it was .0005"/.0006" out of round, but the other dimensions were fine. The part must be accurate within .0001". This was with breaking the circle geometry into 20,000 straight segments. Line segments is what was recommended by our reseller. Prior to that we tried I's and J's with poor results. With all the options available it is hard to have a place to start. MotorCityMinion maybe you have found some answers since posting about your S56, or does anyone else have suggestions?

 

Even if you have the Moire scales on that V56i, holding .0001 for circularity accuracy is going to be very difficult. Check the report that came wth your machine from the ball-bar test and I will bet that you will not see accuracy of .0001 Makinos typically have reversal spikes at the high points of the axis which will cause slight irregularities. For the ultimate accuracy use G5 P10000 M252 . Whether you use arc commands or linear code, your Makino will give you the same result. The reason Makino recommends short linear code is to take away the "thinking" that the control must do to calculate arc centres. On 3D surface models, this will produce great results at high feedrates. On 2D machining, it will have no effect at all. I have 8 years experience using V56 and S56 Makino's.

 

Carmen

[Joe788]

Carmen, how accurate would you expect to cut a circle on a V56i? I'd be disappointed in any new Japanese machine that couldn't do at least .0002

[GoetzInd]

I've cut bores on an A51 with roundness to .0001 according to our CMM......

 

 

Mike

[Guest CNC Apps Guy 1]

FANUC machines like piles and piles of code. Siemens (and presumibly Heid as well), not so much. The Siemens has COMPCAD.

[Redfire427]

Carmen, how accurate would you expect to cut a circle on a V56i? I'd be disappointed in any new Japanese machine that couldn't do at least .0002

 

On a quadrant ( 90 degree arc ), you should be able to hold .0001 The problem arises on full circles. As I mentioned earlier, the issue I have seen on the Makino's is reversal spikes, meaning, the arc has a little bump ( high point ) at 0,90,180,270 degrees where the servo motor changes direction. All Makino's come with a ball bar test report in the rear cabinet that shows the test from the factory.

[huskermcdoogle]

FANUC machines like piles and piles of code.

 

Assuming you have HPCC or AI-NANO? Or will they process these well in G08 P01? What age, and what model controls?

 

In HPCC coming from a Data Server, which method will potentially make a Fanuc process movement faster? Lots of short line segments, or lines and arcs filtered? How long of line segments would be suggested? Of course the latter probably depends mostly on what type of geometry you are cutting, but for general surfacing or large curved surfaces what type of segment length would you use?

 

Husker

[MotorCityMinion]

One thing I have noticed with G05 P10000 on the S56. I project curves to a plane which are used to drive a Blend tool path or boundaries. I have to reduce the number of entities in those projected curves or else the machine stumbles, especially with blend since the tool path is generated from the shape of the drive curves. During projection, what would appear to be one straight line becomes multiple splines. Same with projected curves which can become unruly. I create node points, end points, delete any dupes, then recreate straight line segments. Next I use a spline function to recreate the curvy geo and use the new entities to drive my path. I know this sounds like a lot of work, but using the arc filter will take some liberties with the tool path (crude it up) so I avoid it when I can and the Makino runs smoother with very short line segments. I also avoid check surfaces when I can as this can cause spikes and unnecessary retracts. Instead, I'll create a dummy drive surface either flat or normal to the geometry, to help keep the tool down and the tool path smooth, and include those surfaces in the drive selection as well. Sharp corners should always be avoided as well. Put fillets in there when possible.

 

 

 

 

"The part must be accurate within .0001"

 

I don't think I would attempt that on a mill using interpolation. I'd even be skeptical seeing a jig grinder attempt that.

[huskermcdoogle]

I don't think I would attempt that on a mill using interpolation. I'd even be skeptical seeing a jig grinder attempt that.

 

Yeah you certainly can't be capable from a statistical standpoint on any mill to that tolerance.

 

 

Husker

[CarbonCAD]

We should be there now, but as Goetzlnd said "roundness to .0001 according to our CMM......"