Our machine (Mikron VCP600) is capable of 0.6 g's acceleration. Top of the line high speed machines are doing 1.5 to 2.0 g's. These machines are very scary to watch. Mikron achieves this performance with water cooled motors and leadscrews. Some manufacturers are using linear motors (no leadscrews required).

Most newer high speed milling machines will automatically reduce speed during direction changes to maintain a user specified tolerance. This results is an actual cycle time that is longer than the backplot estimate. The highfeed machining function in Mastercam takes care of the feedrate changes within the program. This is especially helpful if your machine does not do this automatically.

Sorry, I see that you said you were set to incremental.

You must set the depth in the toolpath to "incremental" and "0". Check this before messing with the post. An "absolute" depth setting results in all holes being the same depth as the first.

Programming for older AGIEs is tough. Hard to find a really good 100% solid post. 2D contours required the first and second lines of gcode to be inverted and the contour exit needed dummy moves related to cutter comp. 4-axis programs are a total nightmare. All current AGIEs use the AGIEVISION control. Gcode formats are very simple (standard ISO). 4-axis programming is especially simplified.

Both manufacturers produce very high quality machines. They are the leaders in the EDM field. Both companies are owned by the Georg Fischer Group. You will not be screwing up by buying either of these. We use Agie EDM equipment exclusively. Agie is regarded by most as the "best" machine available especially with regards to accuracy.

Everything in this thread applies to electrodes regardless of material (copper, graphite, copper tungsten, etc.)

In Summary: Scaling is Bad - works for shrink allowance in mold but not for electrode undersized. To make an elecrode for a mold using part geometry, first apply scaling to allow for shrink then apply surface offseting or negative stock for undersizing. Order is important - Do not offset for undersize/spark gap then scale for shrink. Negative Stock is the preferred method resulting in a consistent undersize normal to all surfaces. Fudged tool descriptions give correct results and work around the undersize cannot be greater than tool radius issue. To obtain correct dimensions in the EDMed cavity using electrodes produced this way requires a spherical orbit. Various EDM manufacturers have names for this (AGIE=equimode, Charmilles=3D-ORB, etc.). These 3D Spherical orbits make the cavity larger than the electrode as measured normal to the surfaces (the same way Mastercam undersized it). Other orbits such as circular, cylindrical, 2D vector, 3D vector, polygon, etc. will not yield correct cavity dimensions. Some new CNC Sinker EDMs Do not have a spherical orbit, most old CNC machines do not and ALL manual machines retrofitted with orbiting heads do not. Keep this in mind if you know you are doing it right in Mastercam but your cavities are not right. Cutting a 3D shape with a non-spherical orbit requires the shape of the electrode to be distorted. For example a circular or cylindrical orbit requires all electrode geometry to be undersized or moved in the top view (X-Y Plane)only. No easy way to do this most of the time. The part has to be completely remodeled. Ouch!

I am running an ATI Fire GL2 w/ Win2K. Terrific with Mastercam. Cant't run games. No Win9x drivers either. Anybody else using a Fire GL card?

Try Tesco Technologies - they import Jabro tools. Talk to ED or Rob. If they can't help you they will point you in the right direction. I have successfully used 0.3mm tools from them for hard die milling. Their number is 877-908-3726.

Does the machine use glass scales or encoders? I had a machine (sinker EDM) do the same thing due to dirty glass scales.

I have not looked at your file, but I usually get better results using very tight tolerances. Calculation times will be increased considerably.

"High Speed Machining" is light cuts at very high spindle speeds and feedrates. On a capable machine the metal removal rates are impressive. I can rough out a pocket with a 1/2" Ball cutter using HSM techniques faster than a 1 1/2" insert cutter using conventional methods. The roughed out cavity is much closer to finished shape since the smaller cutter fits into more tight areas (reducing the amount of semi-finishing). A good starting point for roughing in hardened steel is 5% depth of cut and 5% stepover with spindle speeds ranging from 15,000 (1/2" cutter) to 40,000 (1/8" cutter). Feedrates around 350 ipm. Finishing stepovers of .001 to .003 at 30-40k RPM at 200-500 ipm work well. Mirror finish - no handwork - .0002" accuracy. Machines designed to do this kind of work well have heavy stationary bases, lightweight moving members, and powerful drives. They are capable of very high accelerations. The best machines can accelerate at 1 to 2 g's. Acceleration specs. are an indication of how much time the machine will spend at the high programmed feedrate rather than the slow feedrates the machine will use to maintain cornering accuracy.

The best high speed machining data I have found is published by FRAISA. They are a European cutting tool mfg. with offices and distribution in the U.S.

We have a Mikron VCP600 with Heidenhain TNC 426 and output Heidenhain code (.H files) from Mastercam. We are high speed milling graphite and hardened steel with a 42,000 rpm spindle. I modified the generic Heidenhain post (mpheid.pst) to suit our needs. Fixed some bugs related to arc output. The post determines if we are cutting graphite or steel based on the tool number and outputs the appropriate codes (dust extraction and airblast for graphite and oil mist and oil mist extraction for hard die milling). Our other mills use ISO code. Our operators have had no trouble adapting to Heidenhain. I have been told but not verified that Heidenhain code is processed faster by the control. This would be a consideration in high speed cutting.

Use "Tool Plane" if you wish to transform your pattern using multiple work offsets (G54, G55, etc.). I prefer "Coordinate" transform. It has fewer limitations and simplifies things at the machine (only one "zero" to set). Does anyone know if it is possible to make "Coordinate" the default setting in toolpath transformation? I have made a number of bad toolpaths by not being careful to check this.

Make sure you select "Coordinate" instead of "Tool Plane" as the transformation type. The default is "Tool Plane". Does anyone know how to change this default?

Are you sure Zeiss is not available? If at all possible get a Zeiss w/ Calypso software. If you need to check free-form 3D surfaces add the Holos software. If your budget allows get a scanning machine. Mechanically the Zeiss is equaled only by SIP and Leitz. The Zeiss software is far more powerful and user friendly.

The main features needed for successful HSM are: Spindle - you need 30k+ rpm. Beware of high rpm/low HP spindles; however, high rpm/high HP = money! HSM spindles live hard lives. Check out the spindle warranty and replacement cost before buying anything. Some mfgs. have a spindle replacement program. Acceleration - usually expressed in g's. Above 0.5 g's is good. Top of the line machines are 1 to 2 g's. This is a measure of a machine's ability to rapidly slow down entering a corner and rapidly speed up exiting the corner. High G machines spend more time at programmed feedrate rusulting in shorter cycle times. High G machines tend to be fairly massive with heavy stationary components and lightweight moving components. Control - Look-ahead buffer and block processing speed are important. Automatic Accel/Decel based on a contour tolerance simplifies programming. We use a Mikron with 42,000 rpm 18 hp spindle and 1 g acceleration. We cut graphite, steels up to 60 Rc, aluminum, and copper-tungsten.

Many newer high-speed mills will automatically slow down in order to maintain accuracy and fine detail in sharp corners and small radii. The actual feedrate will be reduced any time there is an abrupt change of direction. A tolerance is usually called out in the NC code and the machine will decelerate as required to maintain the tolerance. Actual cut times can exceed Backplot estimates by 15% to 100%. We are cutting steel and graphite on a Mikron HSM with 42,000 rpm at speeds of 400 ipm. We have become fairly good at taking the Backplot time and considering the amount of detail in the cut and "guessing" the actual time.