Mastercam High Speed Toolpaths

[Troy Gossett Indepak Inc.]

Roger, Thank you I haven't had it happen recently so I don't recall where the gouges were exactly. I'll watch for it though. Yes I'm using the arc filter as I do with all other toolpath types.

 

Gcode, Thank You I don't know why I didn't see that before... I usually use feed plane and not retract as our plates here are usually squared ahead of time. So the max retract illistration looked like it was retracting to far. I should of read it instead of looking at the picture, oh well it makes sense now.

 

Troy

[Fred @ Slate Industries]

Like its 2d cousin Rest mill

High speed Rest Material is still lacking the function end of it.

I know the work around is to save your roughed file as an .stl then bring that in but really

there both not there for me.

 

Rest mill I have to boundry off sections instead of having one huge number crunch.

[Roger Peterson]

Good catch gcode, I missed the "minimum vertical retract". The devils in the details, and as gcode said you can definately get gouges using this retract macro as well.

[Smit]

Do the gouges show in vericut when you process the G code?

[Saultspics]

The biggest problem I have with HST is the finish toolpath is reseting the stock from 0 to .050".

 

Has anyone had this problem?

[beej]

I use full vertical retract every time and I have NEVER had a gouge. in the high speed paths. I use them all day everyday in what I do and they work great. (aside from taking a while to generate)

[Troy Gossett Indepak Inc.]

Stephen yes that happens here too, I have found you need to hit the apply button on each page before going to the next, or you lose it.

[Fred @ Slate Industries]

Today was a good day! HST was o.k. with my model

And 3 HST paths later another Kick a$$ electrode was machined in a heart beat !

Awesome...

[gms1]

Im having issues with these toolpaths too and its stuff I cant figure out.

I can tell it to do a core roughing and leave .01 on the walls and 0.00 on the floors and it still cuts to .0001 to .0005 above the actual finish of my part. I like to also use profile ramp entry and set the entry feed to "feed rate" yet it still outputs my rapid feedrate no matter what I change.

[Matt Berube at Ferron Mold]

Regarding the cut depths...

 

I tried to report that as a bug a long time ago but it was rejected if I recall correctly.

 

With the old toolpaths, what you specify for the max depth is what the max depth actually cuts. With these new ones, it is allowed to vary by whatever your tolerance is set to.

 

Regarding the feed rates, I would send that to QC...

[gcode]

Before sending the feedrate problem in as a bug,

try posting the offending toolpath with a default machine. It may be a post issue, especially if the post has been upgraded a couple of times or is heavily modified. A hinky machine definition can cause this as well.

 

[ 04-21-2007, 09:52 PM: Message edited by: gcode ]

[gms1]

quote:

---

Regarding the cut depths...

 

I tried to report that as a bug a long time ago but it was rejected if I recall correctly.

 

With the old toolpaths, what you specify for the max depth is what the max depth actually cuts. With these new ones, it is allowed to vary by whatever your tolerance is set to.

 

Regarding the feed rates, I would send that to QC...

---

Which tolerance does it set these depths to? My post settings or is it the minimum step down?

[Matt Berube at Ferron Mold]

The situation I was referring to happened nearly a year ago. I haven't seen it lately so I am not positively sure that it is still functioning the same.

 

I was trying to restrict which areas were to be cut by specifying "cut depths" which should have eliminated certain cut levels. Mastercam was making the cuts anyway and "gouging" the surface by whatever was allowed in my filter / cut tolerance.

 

This was a High-Speed Horizontal area toolpath.

[andrewgore]

When mastercam first came out with their HST's, I switched over to using them exclusively. I did this mainly for the fact that I could switch the type of toolpath, without having to create a new operation.

 

The only time I have found to have gouging is when I set my retract heights too low. I run probably .020" above a part at 1000ipm. My parts aren't huge, but I like to keep myself on my toes.

 

The thing you have to be careful with things, is if you start off with a core roughing operation, If your stepdown is something like 4mm with an 80% stepover, you need to IMO make sure that "add cuts" is enabeled. Basically if your final depth doesn't get into that 4mm stepdown, there is a chance that there may be 4mm of stock at the bottom of your part left. With add cuts enabeled, I usually put a min stepdown of about 10% or less of my max stepdown. This ensures not too much stock is left on the tops of anything, and the floor is to the depth that I specify.

 

This also holds true for tops of any flat. If it isn't within the max stepdown (and "add cuts" is not enabeled), there is a good chance for gougeing.

 

Cool now too that there is a graphical interface for the trochoidal motions as well. My tools last much longer, and while I do generally wait a little bit for a toolpath to generate, it has usually been worth it. Downside to these methods is that in Verify, they go process rather slow.

 

One thing I would also mention is that I make sure I always hit the "apply" button after I'm done editing each page of the HST menu. I had in the past information not be saved, and I had to go back and re-enter numbers. No real biggy.

 

I've finally also gotten some of my machines own smoothing filters figured out (still scratching my head) and messed around with my post a bit in hopes to make things move faster and smoother.

 

I will say that the HST's def. helped on an aluminum fixture I made awhile ago. Using 12mm bull nose, with 12mm stepdown, and IIRC, 30 or 40% stepover running @ 600ipm, the trochoidal paths make it sing like a bird (and look like a snow storm). If you are having troubles with the toolpaths, it is more than likely a setting that needs to be adjusted. It took me a while to figure out exactly what works best for me, but once you do, making toolpaths is as simple as selecting geometry and hitting the OK button.

 

Hopefully that helps someone if they are having gouging situations.

 

Andrew

 

ps, I feel like I can actually trust my tools at what the manufacturers suggest for cutting speeds. They will hold up!