roughing programs

[mjs97]

we build molds and i use x5 to program. when roughing a mold i use rough pocket and usually set stepover to 75% of tool dia. using a flat inserted cutter, i still seem to get islands left behind. i change to 60% and its better however still once in a while leaves island. is there any settings i can change so it will check for islands left behind? program takes longer when only stepping over 60%, so im getting a little frustrated.

 

i tried hstp area clearence, and that path took 2 hrs longer than the rough pocket, so i gave up on that. might be more settings im missing there also. i changed a few of them, however didnt make much difference.

 

i am not impressed with any of the high speed toolpaths. it takes forever to figure out what they do and changing settings and still dont like the result.

 

any advice?

 

thanks

[Tony35]

if there is a radius on the tool MC wont account for it (which sux) i have got some xxxx left behind too

the high speeds work good just keep playing with them

[peon]

I have not found a way to avoid the islands either. It's embarrassing when the boss and the men on the floor are asking why I can't machine with an adequate stepover. The pocket toolpaths are just plain inefficient and it has been that way for a long time.

[K2csq7]

mjs, Post a screenshot of what the pocket looks like, Tell us how deep & what tool you wanna use. Your right about the time it takes to learn the new toolpaths, but they do work really well once you know how to do it.

 

Welcome to the forum!!

[mjs97]

is there any suggestions on how to learn these high speed toolpaths other than trial and error? takes alot of time that i dont have. you know how that is.

 

thanks

[Guest]

Check with your reseller.

 

I know we offer 2D HST seminars. I just did one yesterday

[neurosis]

do a search on google for Mastercam hst webinar and you will find a video that explains enough to get you started.

[Redfire427]

we build molds and i use x5 to program. i tried hstp area clearence, and that path took 2 hrs longer than the rough pocket, so i gave up on that. might be more settings im missing there also. i changed a few of them, however didnt make much difference.

 

i am not impressed with any of the high speed toolpaths. it takes forever to figure out what they do and changing settings and still dont like the result.

 

any advice?

 

thanks

 

If you build moulds, you should be using the HST toolpaths exclusively. To say the area clearance toolpath takes two hours longer is due to improper use of the toolpath. The HST toolpaths will run circles around the old legacy toolpaths. If you are not impressed with the HST toolpaths, then it is only because you do not know how to use them.

 

If you provided me your tool info, I would more than happy to apply some HST toolpaths to your file. Email me the file if you are interested.

 

Carmen

[Goldorak]

the new opti-rough in X5 just kill any other roughing cycle in cycle time and programming time (a single operation rough the entire part efficiently)

 

try it and play with it, once you find the good settings , you will never look back

[Mr. Wizzard]

If it's (HST) dancing around a lot and causing extended time, play with the gap settings, retracts, keep tool down, etc... Also, the 2-d HST work well. I don't have "extra" time to play with them much, either. But, learning the high-speed toolpaths will pay off. I typically don't use pocketing anymore because of the newer options. I've also had small cusps left with simple pocketing toolpaths and it seems that a simple pocketing routine should be easy money. I end up playing with the stepover, like you to eliminate them. Why not play with the new paths instead of fighting the old ones? Once you start, it gets easier and quicker every time you use them.

 

Scrap the old, start using the new.

[Ocean Lacky™]

I build forging dies and use ball mills almost exclusively for cavity roughing. HSM Area Clear and a 3/4" inserted ball nose is my method of choice. With HSM Rest Roughing and an STL from verify, I can go right to semi-finishing with a 1/4" ball nose with out worry. Our productivity has never been better.

 

 

Learn it...

Spend some time with it...

You won't be disappointed.

[mjs97]

ok lets say alum block using opti rough. what would be some good #s to start with? i usually use inserted flats (1.25dia with .125 radius actually) to rough , but not sure how they will handle it taking deep cuts. most of the inserts are 1" tall or so. i am running haas mills.

 

im thinking .5dp with .125 stepover with .075 stepup. just a guess. 50"s per min to start.

 

half my problem is convincing the older operators that this is a better approach. so i want to make sure that im close on my #s the first time.

 

any advice is appreciated.

[K2csq7]

Here's a link to a great database for info on these paths.

Thanks Chris!!!!

[CJep]

Thanks Keith I was looking for that,..

 

I thought it was pinned to the forum?

[K2csq7]

Me 2????

[Guest CNC Apps Guy 1]

I use the HSM stuff about 90% of the time. There's a few instances where the older ones give me closer to what I want, but not too often.

[Jayson Kramer]

I use the HST 90 percent of the time these days to. When cutting cavity's or cores the HST stuff kicks butt.

The HST for the finish is top notch unless you are using a stinking Fadal they give frigin helical arc errors on the HST finish scallop and Waterline.

 

Why would a good mold shop by a Fadal to cut molds is beyond me. Two shops I just programmed for had fadals and they barffed on the HST when onther machines includding the Haas's rocked.

Matsurras love the HST stuff.

Sorry about the rant but the Fadals just kill me.

[rgollar]

Why would a good mold shop by a Fadal to cut molds is beyond me. Two shops I just programmed for had fadals and they barffed on the HST when onther machines includding the Haas's rocked

 

This surprises me because my 1997 fadal kicks to snot out of my 2009 haas when it comes to high speed machining. The haas just chokes up to darn near ridicules times as the fadal just machine with out alot of slowing down. I tried the high speed option on my haas but that didnt really help all that much.

[Jayson Kramer]

what controls are on the fadals. the ones I had issue with were C88 controls the old stuff.

[rgollar]

That is the same controller Im running which is cnc 88hs. Im just trying to figure out what I am doing wrong on my haas to make it such a slow surfacing machine. I am in mo means saying your wrong Im just trying to figure out what im doing wrong with my haas. I even tried set my setting in the haas to rough and turning my radius up to .01 and still no difference.

[Rstewart]

I would set that E value up higher like .015 or .02 on the Haas for Roughing. Works for me....

[rgollar]

Thank you I will give that a try.

[mjs97]

i must not be doing something right. i have 36"x18" alum mold. cavity is about 4" dp in most areas and round in shape. with opti rough taking .5 depth of cut and .125 stepover and .1 stepup it takes 8 hrs to rough out. with old style pocket rough taking .06 depth of cut and 60% stepover it takes 8 hrs. same feedrates. ive tried changing settings but must be missing something.

 

any help is appreciated.

[Goldorak]

what kind of cutter do you use ? thi will make a huge difference

[Goldorak]

play with your setting cuz for a 36 x 18 x 4 pocket with 1.5 radius , cut with a HSS 3/4 endmill . i got just over 2 hours of cutting time

 

my spec is 6000RPM, 160IPM, 2.0DOC, .125 step up 12.5 step over and 400IPM back feedrate (machine max) and .05 microlift to avoid tool drag