Mastercam High Speed Toolpaths

[gcode]

I've been working on a project at work during my spare time I finally got to prove out some toolpaths yesterday.

 

Its an aluminum forging on a 4 axis HMC.

They've been building it for years the old school way with big cutters moving real slow.

 

Aside from poor cycle times, the big cutters also

knocked the part around on the fixture causing

repeatability issues. This was was assigned to me as a proccess improvement effort.

 

I replaced all the big slow cutters with small fast cutters. For example a 2 x 6 in rougher

making 2 passes a 8in was replaced by a 1in long necked rougher making 4 passes at 45 ipm.

 

One high speed tool path really impressed me.

I didn't think it would work, but I tried it

anyway

 

The part has 2 pockets with 1/2" wall and floor fillets. Ears on the forging require the tool to be 3in long even though the pockets were only 1.2 deep.

The old program used a long 1" HHS ball ramping in at 1.5ipm and pocketing at 3ipm. Cycle time was 12 minutes and yeilded very poor finishes requiring lots of benchtime.

 

I roughed this with an Ingersoll 3/4in by .03R 2 flt insert mill, 3 in long with through the tool coolant.

 

I ran it at 5000 rpm ( machine max) and 68 ipm.

It was programmed with high speed core roughing

.08 depth of cut with countor ramping and 400 ipm

rapids.

 

I expected this toolpath to chatter badly and

planned to adjust with feed and speed override

to find the sweet spot.

Much to my surprise, this toolpath purred like a kitten with all oversides at 100%.

 

The pockets were finished with a 3/4 long neck

3 flt carbide ball, using a high speed waterline

on the walls and a high speed scallop on the floor.

 

The old cycle time... 12 min plus bench time

New cycletime 5.5 min and 0 benchtime

 

These high speed toolpaths are cool

[Guest]

As nice as these paths seem to be I find they take way to long to generate. I also have had two gouging problems with them both of those however were being used in transform paths as well.

 

Neither problem showed in back plot or cimco verify but both were clearly in my parts.

 

Surface rough pocket in both cases did not cuase a gouge using the same geometry to cut/

[gcode]

Yes, the proccessing time it too long. For big parts its so long as to make the high speed toolpaths useless.

 

As for the gouging issue, were you using the

highspeed feedrate option for rapid motion?

This stuff was scary at first and some of my operators refused to run it when they saw the

F400. feedrates.

 

I can see how Transform/Rotate could get you in trouble, especially if you're using G0 rapid motion.

 

I run all my gcode through Predator and it has saved me more times than I can count.

[Guest]

nope, I had it set to rapid retract.

 

both gouging issues were in actual cutting moves not retracts. Both violated drives surfaces.

 

When you have to stand in front of your boss and try to explain you don't have a clue why it happened and no one else does either, they were sent in, it doesn't make me want to explore them to much more deeply.

 

I am also at a loss as to why the cimco verify did not show me the rough cut either.

[peon]

I also gave up on the high speed toolpaths. I have to program and operate the machines. Everything I do is in a rush and I don't have time to wait for toolpaths to generate. Although, the high speed horizontal toolpath is useful to me. Some of my larger parts would just choke on the high speed toolpaths.

[Ocean Lacky™]

I use the new High Speed toolpaths daily for Die cavity work. I've seen a "ding" or two, but fortunately in a forging die, we can send it to the welder, .... no biggie .... For my applications, they run flawlessly 99% of the time with decreased cycle times. I haven't experienced a dramatic increase in toolpath generation times. When I do, I can usually trace it back to a faulty surface (we don't have Solids)in the model...fix it, and regen times go way down.

[DavidB]

The HS toolpaths are big drain to process, but the time saved on the amchine is greater.

 

Would be great if we could batch them then process when you go home.

[Roger Peterson]

DavidB, You can still batch process them, you just have to select the toolpaths manually. When I had a real job I batch processed every day. I cannot imagine not batch processing, regardless of how long the calculation times are, there is no way you can compare a faster calculating toolpath to having your pc crunch toolpaths while you are at home sleeping, at lunch, or even in a meeting. Batch processing is something that not many people do, or even know about. But it is something that many, many people could benefit from. I realize that hot jobs come up and you have to deal with them on the fly. But, for the majority of stuff it's not that hard to schedule a day in advance so you can batch process overnight.

 

Batching toolpaths can actually give you better parts. How many times have you told yourself I'd like to see what this part looks like with X toolpath instead of Y toolpath, but you don't because you don't want to wait for it to calculate. Set em up, batch em, compare em... Run the one you like.

[Fred @ Slate Industries]

You mean I'm not the only one ?!

With maintenance due,I told my employer

We need it so that when they Tune,Tweak,Fix

The Highspeed toolpaths we will be all set.

[Roger Peterson]

John, my guess is you have some type of arc output issue between your post and machine. Were you able to identify the line of code that caused the gouge?

[Guest]

Roger,

 

No I did not. The code was just way to massive for me to want to dig through it.

 

I have trouble believing it's a post issue if only becuase of the volume of work I do with this particular post. This on my machine where all my my "critical" work is run through and it is only on this core rough that this has been a problem. An arc issue is not likely if only beacue one of the errors removed and extra .009 along a vertical wall, no arc output there.

[DavidB]

Roger,

I can not see how to batch a HS Toolpath?

 

This is from a surface rough pocket toolpath.

 

Where is the BATCH switch in a HS Toolpath?

[Roger Peterson]

DavidB, like you said there is no "to batch" checkbox in HST toolpaths. But when you create your batch file you can select any file, select one or more toolpaths and hit the arrow to add them to batch file, select another file, select more ops, hit the arrow to add to batch file, etc... Not quite as easy as being automatically selected but it works until they get batch processing added to HST toolpaths. When you create your toolpaths you want batched, set your parameters, hit apply, then hit the red X.

 

 

HTH

[DavidB]

Roger,

When you create the HS toolpath it automaticlly processes how do you stop it from processing so you can process it with a batch file?

 

Thanks

[Roger Peterson]

Set your parameters, hit the apply button, then hit the red X, it will ask you if you want to keep the operation, hit yes.

[Troy Gossett Indepak Inc.]

I had high speed core roughing gouge a part last week. Didn't show up in Verify, showed on the part though. This was a progam with multiple male features rather than pockets.

[Guest]

Were you transforming the tool path at all?

[Troy Gossett Indepak Inc.]

I spotted something today when going through my ops.defaults it reminded me of this topic.

 

In the cut parameters page there is a setting called "Keep Tool Down Within"

This is what the help file says about it:

 

Distance

 

If the distance from the end of one pass to the start of the next pass is less than this distance, Mastercam will not create a retract move as defined on the Linking parameters page. Instead, the tool will stay on the surface and move directly between the passes at the feed rate.

 

% of tool diameter

 

If the distance from the end of one pass to the start of the next pass is less than this distance, defined as a percent of the tool diameter, Mastercam will not create a retract move as defined on the Linking page. Instead, the tool will stay on the surface and move directly between the passes at the feed rate.

 

 

This seems like it could cause the gouging issue if left larger than the Max Stepover(if I understand it correctly) So why is it set to such a high value

by default.

[Roger Peterson]

I've had close to a dozen people send in what they thought were gouges during the running of the core rougher toolpath, it didn't show up in backplot, verify, or metacut. The gouge came from using the minimum distance transitions on machines that do not support it. Dogleg moves don't show up on most any backplotting/verification software so they were unable to detect the gouge until the part was ran. I go through this in great detail when doing training, but people who have not been in for training and don't know the dangers of this try it because it looks like it will run really fast. You will eventually get a gouge. Unfortunately they think the toolpath did the gouge and go back to the standard toolpaths, missing out on all the advantages of HST.

 

Be very careful of using minimum distance transition moves unless you are posative your machine interpolates them, or you output them as feedrate moves.

 

 

HTH

[YoDoug®]

quote:

---

output them as feedrate moves

---

That's how we do it here. The machine actually runs smoother that way. However our parts are so small that the difference between full speed G01 and rapid is hardly noticeable.

 

Also Vericut, if set-up properly, will show dog-leg moves in rapid.

[gcode]

Most machines do not rapid in a straight line.

Some have a parameter that forces straight line

rapids and its safe to use minimum retract and rapid for these machines.

All others should use the G1 rapid or the full retract option. Otherwise you will gouge your part sooner or later.

 

another expample of these high speed toolpaths

that I programmed a couple of weeks ago.

 

a 6in deep pocket in steel on a big horizontal machining center

 

Old school-- Ø2.00 x 6in LOC 8 flute rougher

2hrs 45 minutes of shaking and rocking and breaking $500 endmills

 

Mastercam HS and a Mitsubishi 3" high feed shell mill on a 6in long arbor

890 rpm x 120 ipm x .059 doc

45 minutes of buzzing and blue chips flying 30 ft.

I would not have believed it if I hadn't seen it with my own eyes. It did the whole pocket without

indexing inserts.

[Troy Gossett Indepak Inc.]

That isn't what has caused it here. I use Minimum Vertical Retract. So the machine should always move to the z clearence plane and then across to next position. I still have gotten random gouges that can't be explained by tolerances, .035 stock to leave should be plenty with a 3/4 carbide cutter in 6061. In my post ^^^above^^^ I described what I think could be causing this, has anyone played with this # either dist, or % what values work for you?

 

The way I read the explaination is that if the next step is less than the number in either of those boxes Mastercam will skip the retract and attempt to follow the surfs(I'm guessing at rapid rate if that is your selected output) to the next cut entry point. So for example if you set it to Keep Tool Down Within, Distance = 0.0 it will always retract and then move to next location... Right???

[Carl Hessig]

I've been using them since they came out in beta and have not had any gouges.

Switched from using sandvik cutters to Mitsubishi 2" AJX for Core roughing and 3/4" AJX for Rest roughing. I have seen cutting times for roughing out P-20 cavity and core blocks drop from 5 hours per block down to 30 min. per block.

The high speed finishing paths do a great job on hardened steel.

Processing times are not that much different.

I still use a mix of new and old cutter pathes when cutting electrodes.

[Roger Peterson]

Troy, in the standard surface machining toolpaths you can choose to gouge check the transition motion or not. In the HST toolpaths ALL transition motion is gouged checked with no way of turning it off. I have not seen any gouges that I could attribute to the gap/transition motion. I don't recall encountering a gouge that was caused by anything other than the minimum distance retract.

 

Are your gouges happening at ends of cuts?

 

Are you using the arc filter?

[gcode]

quote:

---

Minimum Vertical Retract. So the machine should always move to the z clearence plane and then across to next position

---

Minimum Verrical Retract can gouge or crash if your machine does not rapid in a straight line.

 

Take a toolpath that gouged, change it to

Full retract or better yet Minimum Distance

and check Output Feed Moves.

I'll bet you don't get a gouge.

 

The bottom line is...

If your machine does not rapid in a straight line,

you should either use Full Retract or have

Output Feed Moves checked