High Speed Waterline

[g huns]

First, thanks to CNC for adding these high speed paths for those of us too cheap to buy Cimco HSM. They look pretty cool, but I just did a path using the waterline path and used a -.0025 for stock to leave on my drive surfs. Well it wants to cut away a feature that is one of the drive surfaces....

 

This is with 0 for stock to leave

 

Now if they don't work with -stock, that's ok. Or maybe I'm missing something, the new pages for the high speed paths take some getting used to. Just wondering if anybody else noticed this.

[HevyMetl]

I won't get mine loaded until Friday. Greg keep shaking this thing out for me. I hope to give this thing a run for its money by the end of next week. Lots of trods and cavities to cut.

[Bill]

I have a lot of trode modeling to do, but I should be cutting by Friday too.

 

Can't hardly wait.

[Chris Rizzo]

What do you have selected for your drive geo? Try selecting the entire model, but limiting it to those features via depths settings.

 

I've been playing with HST pretty extensivly for a few weeks (I've found some stuff with waterline too), if you want send it to me and I'd be happy to take a look.

 

hth

[g huns]

The entire model is selected as drive, used the depth settings. This is a trode so I went back and just changed the cutter diameter. The toolpaths HST makes look neat, and I'm sure in steel they will go easier on cutter, but on my machine they are not faster. I have a Fanuc 16 control with HPPC and it really slows down with the arcing on and off the part, to many splines, not enough arcs. Not sure if there's something to tweak to get more arcs out of it.

[Scott Sizemore]

We have called Fanuc on arc filtering and Fanuc told us to send the entire program out as linear. We were told that arc filtering on our V55 would slow down it's performance by 20-30%. They were right. We pulled all arc filtering on any of our Fanuc controllers. So maybe try taking your filtering off all together.

[gcode]

quote:

---

We were told that arc filtering on our V55 would slow down it's performance by 20-30%

---

Are you referring to the arc filter setting in

Mastercam toolpaths or some parameter setting on the control?

[HevyMetl]

We were told the same thing by Makino. We strictly output linear movements to our SNC64, and the programs run better. Surface finish actually improved over arc filtered paths. I have our tolerance set 1um or .00004". Paths do get incredibly long.

[g huns]

Where do you set it at?

[Scott Sizemore]

Yes I am referring to arc filtering in MasterCam. I turn off all arc filtering in MasterCam. However for tool compensation purposes we do output arcs for bushing holes, anything 2D, etc.

[HevyMetl]

In the post I am not sure. Camdude set it up for me when he was still at Prism Engineering. Maybe he is monitoring and will answer.

[g huns]

I wonder if some the control parameters related to the HPPC need tweaking. When it makes several very small movements it does vibrate a little. Is there a total tolerance setting in the control parameters?

[g huns]

Ran a path with filtering off, 14 min 58 sec. Same paths, with filter 2:1 and same total tolerances as no filter paths, 13 min 57 sec. Finish looks the same.

[HevyMetl]

On the machine or through backplot? What was your cut tolerance set to on your finish parameter page? Is you post outputing 5 decimal place output? These little thing made a difference in how the machine ran for me. It still has feed slow downs in spline sections, but arcs fly. Makino blames this on MC output, I don't but it completely, but all of this has been covered before.

[g huns]

That's on machine time. My total tolerance was .0001 for a rough pass, and .00005 for finish. Nope I'm only outputting 4 place, duh I missed that. My old post did 5, but I switched to MPmaster and it spits out 4. I'll tweak that and give it a try.

[g huns]

Ok I'm stumped. I remember that changing from 4 to 5 place decimal in my old post was pretty simple, but I can't get it for the MPmaster. Got the mtol at .000001, changed x, y, and z position output under nc output variable formats, still get 4 places.

[HevyMetl]

It is one of the format statemets. I am pretty weak in the post area, but I think this is the section that controls the decimal place output.

 

# --------------------------------------------------------------------------

# Format statements - n=nonmodal, l=leading, t=trailing, i=inc, d=delta

# --------------------------------------------------------------------------

#Default english/metric position format statements

fs2 1 0.7 0.6 #Decimal, absolute, 7 place, default for initialize (

fs2 2 0.5 0.3 #Decimal, absolute, 4/3 place

fs2 3 0.5 0.3d #Decimal, delta, 4/3 place

#Common format statements

fs2 4 1 0 1 0 #Integer, not leading

fs2 5 2 0 2 0l #Integer, force two leading

fs2 6 3 0 3 0l #Integer, force three leading

fs2 7 4 0 4 0l #Integer, force four leading

fs2 9 0.1 0.1 #Decimal, absolute, 1 place

fs2 10 0.2 0.2 #Decimal, absolute, 2 place

fs2 11 0.3 0.3 #Decimal, absolute, 3 place

fs2 12 0.4 0.4 #Decimal, absolute, 4 place

fs2 13 0.5 0.5 #Decimal, absolute, 5 place

fs2 14 0.3 0.3d #Decimal, delta, 3 place

fs2 15 0.2 0.1 #Decimal, absolute, 2/1 place (feedrate)

fs2 16 1 0 1 0n #Integer, forced output

fs2 17 0.2 0.3 #Decimal, absolute, 2/3 place (tapping feedrate)

[g huns]

That's a little different than mine. I'll give it a shot. Can you show me what your Toolchange / NC output Variable Formats look like?