High Speed with SGI

[Brian_99]

I have a Makino V77 with SGI and was reading previous threads about not filtering programs. So I decided to test this on my machine and came up with the opposite results. My cycle times were actually longer using an un filtered program like everyone was saying to use. Any clues as to why this would happen?????

[HevyMetl]

You must set your part and tool path tolerance very low. I used .00004, and never filtered.

[MLS]

I would guess it depends on how many points you have. If your cutting tolerance on a complex surface is extremely small, the machine will have to adjust the acc/dec more often. Consider going a bit under your tolerance requirement for the surface without overkilling it. I would use filter to eliminate the points where they don't have any purpose.

 

In 3 axis cutting, there is very little need for the extra points. Once again, give it what is necessary for the tolerance you desire, using filter to dictate this.

 

IMO the place the extra points would be a benefit is in multiaxis toolpaths in the areas where there are vector changes, that is swarfing and cutting normal to the surface. I still tend to filter instead using the point generator on vector so I only get alot of points when the toolaxis is actually changing.

 

HTH

[Brian_99]

I did have the tolerance at .00005 which is the lowest mc says you can enter

[Tony35]

[mild hijack]

 

quote:

---

using the point generator

---

mls

is this in 3 axis toolpaths too?

 

i would like to get all points for my makino sgi

what would you guys do if it was a contour "break many pieces"? or something else

 

[mild hijack off]

[MLS]

No tony, just in the multiaxis toolpaths.

 

If you are driving a line, there is no advantage to have more than 2 points. It would only be of benefit in 3-axis when driving splines or swinging arcs in point to point instead of circular interpolation in which case your cut/filter tolerance will dictate how many points are generated/remain.

 

If I understand the SGI correctly, the control will establish a spline within the parameters set in the control through a set of points in the gcode(your program). If you had 20 points along a line that would only require 2 then it would build a spline with allowable deviation on each point hence causing the machine motion to potentially NOT go in a straight line. Kinda counter productive in my mind.

 

The control does not necessarily NEED more points in situations like that, it will just manage it much, much better than other controls without the feature.

 

BTW supposedly the SGI will calculate point to point circle motion better than interpolated circle motion.

 

Surfacing toolpaths should be the same. If you are kellering a flat surface with a small radius at the end, there is no advantage to having the extra points on the flat area of the surface(It should drive lines). The radius area would benefit with extra points, the flat area would have the potential to hinder.

[Tony35]

mls

what i should of said about the "contour" is that the contour is all arcs. so if i understand this correctly then points would benefit to keep the feed up?

[MLS]

That is what I have heard Tony, but I have not really tested it so I can't say for sure. The idea does make sense though.

 

I think the best way to output points instead of arcs on 3 axis toolpaths is to change your control definition so it does not support arcs. I am not sure however how you control the chordal tolerance for the post when it changes it from an arc into point to point.

 

I know the NCI file is output with arcs regardless. Maybe one of the mastercam post guru's could point you in the right direction as far as that goes.

 

HTH

[Tony35]

thanks for the input mls

 

i am still trying to get this figured out of when to use it and when to not

[Mark H]

I agree, the more endpoints, the more the controller has to process and accdec for each point. With more points, it will slow down.

 

What I do with my Makino S56 with SGI (3 axis)...

 

I use arcs and turn on the filter since it verifies much faster that way (and makes a smaller MCX file.) However in the controlmachine defs, I turn off arc support. So no arcs in the NC file.

 

One side note, if you are seeing facets on the finished piece (especially in circle toolpaths) go in to the MDCD Tolerances and tighten up the tolerances. Specifically note the Chordal deviation tolerance. (see below, taken from the help file)

 

NC percision

Motion tolerance. This is used in the post to determine the precision of the machine tool. It should be equal to the smallest linear step distance on the machine tool. Use the Truncate option to control whether values are truncated or rounded. The value of this field sets the mtol post variable.

 

Chordal deviation

Mastercam uses the chordal deviation for arc break up and line break up post processor routines. The value of this field sets the chord_tol post variable.

 

Deviation of vector endpoints

Deviation of vector endpoints is used when evaluating a normal. The value of this field sets the vert_tol post variable.

 

General math functions

This is used by intersection and fsg post processor math functions. The value of this field sets the xtol post variable.

 

One final note, the more you tighten up the tolerances the larger your NC file will be.

[Tony35]

mark h

what do you have your chordal deviation set too .00005?

 

the size of the programs is not an issue i trip them off a ata card

[Mark H]

Yes 0.00005 (inch) is what I have. Originally it was 0.0001 or 0.0002 and the surface finish was faceted especially when cutting aluminum. On stainless steel it wasn't as noticeable.

 

edit

Oh yeah one other thing - the tighter the tolerance, the longer it takes Mastercam to process a toolpath.

[Tony35]

thanks mark h

[MLS]

Hey Tony.

If you try it out on the machine, how about posting some feedback?

 

I am kinda curious as to how much improvement you get time wise by eliminating arcs in addition to the degree of which it comes out faceted.

 

[Tony35]

mls

sure when a job pops up next for it. what i have seen so far points are better for keeping up the feedrate with SGI on M250-M254, now that i know how to get the points finer i should be able to fly through them

 

i will keep ya posted

[Tony35]

mls

i got a chance to try all points on a cam curve

i took the geometry and broke many pieces (.001 long lines) to rough the slot i used peel mill and the feed was at programmed feedrate 81 ipm when i semi finished the walls the feed was only at 20 ipm not 81 ipm it could only process the points so fast but it did look good i need to have a very good finish on the cam curve so i am going to hard mill finish it and hopefully all the points will benefit when i milled out my clearance slot (spline) i got the programmed feedrate but was faceted a bit the machine ran very smooth with sgi and all the points it seems to depend on the geometry and what you are trying to do in some cases points are faster in others arcs are better

 

any other input is welcome

[MLS]

.001 lengths, Wow!

 

Thanks for the update Tony.

[Redfire427]

Do yourself a favor and take the high speed machining course at Makino in Auburn Hills, MI or Mason, OH. They will help you to understand why a linear code file WILL run faster on the machine. The RISC processor has a 1000 block look ahead to calculate acc/dec times, etc.

Part of the problem is the way in which Mastercam outputs its points. Powermill has a point distribution function that allows a machine like Makino to perform at its best. I believe Mastercam will have a function similar to this with the release of X4 which should help cycle times as well as surface finish.

 

If you want your Makino to perform better during roughing operations, use M251 ( high performance mode ) and the machine will be much more responsive. I would only use this mode for roughing. M250 and M252 should be used for finishing.

 

I still have some text books from Makino that illustrate why a linear code file is better. Most new Makino's come with 2 free training credits at Makino's die/molds locations. Trust me.....take the 4 day course. You will learn a lot.

[Tony35]

thanks prosin