Mastercam Hi Speed Toolpaths

[R. Van Winkle]

In Gibbscam they have Volumill as an add-on. It creates toolpaths similar-looking to the tricordial toolpath form Mastercam of old. A tool rep came in today and said the Volumill toolpath takes into account the cutter's engagement and that Mastercam's toolpaths do not.

Is that an accurate statement? 

He also said the air-cutting time of Volumill is about 27%. What is Mastercam's version of this type of toolpath and how does it stack up compared to 27%?

Personally, I cringe when I walk up to a machine and see it using Volumill on alum. 

[nickbe10]

I used to use Volumil when Mastercam first came out with HF toolpaths. I'm now using X9 and I wouldn't bother now, the toolpaths out of Mastercam are much improved and the RCTF is much better than the Volumill output I used to get, and I hear 2017 is better again.....I am regularly machining 15-5 at 200 ipm.

There are a number of ways to control and minimize airtime in MC, and the percentage of airtime is not necessarily telling you how efficient the toolpath is.

[crazy^millman]

Cool glad to know the tool rep is programming day in and day out to much such a bold statement. How many years of Mastercam Experience does he have? How many different machines has he programmed in just the last year using the toolpaths? When he was programming the same part in the other CAM and was using the Voluemill he could show you the tracked and traced results to make that statement?

27% I would like to see on one of the 40 hour run parts I used Mastercam Opti-Rough with that was removing Material at 180 cubic inches a minutes. 7200 lbs of aluminum to 500lbs so using his proven factual process the customer will see a reduction of 10.8 hours per part. Mind shooting me his name so we can pass it on to our customer they will love to see that kind of reduction on the parts.

[gcode]

I've never used Volumill but I can say for a fact that Mastercam dynamic roughing works and works very well.

I have an old X8 Mastercam dynamic toolpath we ran in 304 stainless steel, cutting big windows through the side of  a  barrel with 1.25" thick walls

Old school was high feed cutters, 12 hours for 5 windows + $800 worth of inserts + a blown cutter or 2 if the operator wasn't on top of his game

Mastercam dynamic toolpath ... 1.5 hours and one $350 endmill per part

It was a safe repeatable process too. Push the green button, close the door and come back in an hour and a half.

 

I did another one on a 316 SS layup mold for a carbon fiber aircraft skin.

Dynamic rough reduced the cycle time from 120 hours to 40 and insert cost from $2500 to $250 ( one box of Sandvik button inserts.)

An added benefit was noise reduction.. the old process howled like a banshee and everyone within 50 yards needed hearing protection.

The dynamic toolpath purred like a kitten and threw a beautiful stream of yellow chips about 20 feet into the sky

 

 

[Leon82]

They work great when using a longer endmill . you don't need to worry about it loading up in the corners.

My only gripe with the 2d high speed is if you are roughing and OD of a part with bosses on it , it tends to radius off the part and come back close to keep the travel distance down.

With a back feedrate of 500 or 750 the machine is slowing down to maintain the precision.  On the matsuura I usually go to r5 precision because lower and you start to hear the direction changes in the ball screw.

Our machine with linear motors is smooth a pie though.

[civiceg]

Quote

In Gibbscam they have Volumill as an add-on. It creates toolpaths similar-looking to the tricordial toolpath form Mastercam of old. A tool rep came in today and said the Volumill toolpath takes into account the cutter's engagement and that Mastercam's toolpaths do not.

 

Kind of. Volumill will adjust the feed-rate based on external/internal arcs. Mastercam has a modifier in the filter in 2018, in the 2d contour tool paths to adjust the feedrate on arcs, I did not see it in any of the Dynamic tool paths however.  I still think machines achieving the actual programmed feedrate is more of a problem than not adjusting the feedrate for Arcs. One extremely talented guy on here was working on a post to make the adjustments for arcs, but Mcam doesn't really have it supported IMHO. 

Quote

 

 

He also said the air-cutting time of Volumill is about 27%. What is Mastercam's version of this type of toolpath and how does it stack up compared to 27%?

Personally, I cringe when I walk up to a machine and see it using Volumill on alum. 

 

I think that is solely dependent on what features are being cut. I would be interested in where the 27 percent came from. A boss will have less air cuts if the stock is symmetrical than compared to the same boss when the stock is not even on all sides. Ex. a rectangular boss out of rectangular stock vs. a square boss out of rectangular stock.  

[civiceg]

Quote

27% I would like to see on one of the 40 hour run parts I used Mastercam Opti-Rough with that was removing Material at 180 cubic inches a minutes. 7200 lbs of aluminum to 500lbs so using his proven factual process the customer will see a reduction of 10.8 hours per part. Mind shooting me his name so we can pass it on to our customer they will love to see that kind of reduction on the parts.

I think he was saying that the total aircut time for an average volumill tool path was 27% of total time, not that its faster than Mastercam by 27%. 

[crazy^millman]

47 minutes ago, civicegg said:

I think he was saying that the total aircut time for an average volumill tool path was 27% of total time, not that its faster than Mastercam by 27%. 

Hard to get what it was meaning from the way I read it, but you could be correct. Was hoping someone found a way to do better than I was doing.

[R. Van Winkle]

15 hours ago, civicegg said:

I think he was saying that the total aircut time for an average volumill tool path was 27% of total time, not that its faster than Mastercam by 27%. 

Yes, that's what I was saying. Total air time cut = 27%. NOT that it was 27% faster than Mastercam. But Ron is correct in that the rep does not program day in and day out and probably is more clueless than clued when it comes to toolpaths.

Thanks for the input. I think it's time to have a Mastercam rep bring their laptop here and do a side-by-side vs Gibbscam on one of our parts that we haven't programmed yet.

[BenK]

27% air cutting time is a lot. He clearly doesn't know what he is talking about. That percentage would change based on many factors, part geometry and programmers ability to manipulate the path being the top ones. The two paths, while comparable, are very different. How they calculate is the biggest difference. I use the controlled engagement toolpaths all the time in aluminum. When you apply them appropriately they can save you a lot of time. Other times they don't help and its up to the programmer to determine weather or not to apply them in any given situation.

[Jayson Kramer]

6 hours ago, R. Van Winkle said:

Yes, that's what I was saying. Total air time cut = 27%. NOT that it was 27% faster than Mastercam. But Ron is correct in that the rep does not program day in and day out and probably is more clueless than clued when it comes to toolpaths.

Thanks for the input. I think it's time to have a Mastercam rep bring their laptop here and do a side-by-side vs Gibbscam on one of our parts that we haven't programmed yet.

So you are not a Mastercam customer now? or you are but you need someone that knows the system better to program it against the other.

I wonder if they have mad any improvements to the Volumill tool. it used to be an add-on for Mastercam at one time. Just like HSM paths from Autodesk started as a option for Mastercam.

[David Colin]

To answer original question : Mastercam HST control tool engagement angle (as almost all dynamic toolpaths from any CAM). In Mastercam toolpaths parameters, you set a radial engagement but Mastercam will internally calculate equivalent engagement angle and will use that to generate its toolpaths (IMHO this info should be added in GUI).

Dynamics toolpathing goal is to maintain a constant hm value for each move during toolpaths. There is 2 main ways to achieve it: maintaining a constant tool engagement angle for every point in toolpaths or adjusting feed according to engagement angle.

I used Volumill a few years ago with MastercamX3 addon then with stand alone Nexion versiin but it's probably been greatly improved now. I d say Volumill 'mainly' use engagement angle to generate its toolpath (but not only) then adjust feed to maintain hm.

Mastercam is tool engagement all the way. This is why in tighter corners it almost generates spring passes as radius toolpath is near tool radius (perhaps it should lightly increase tool engagement angle and reduce feed in that circumstances? It s up to CNC to experiment and check what is more productive or will offer a better tool life). I still dislike the way it manages first pass on outer corners of a square stock (it seems to overload tool increasing radial engagement) but if you check it, you will see it maintains tool engagement angle. I also checked Mastercam dynamic toolpaths with Vericut Optipath, asking it to maintain chip thickness (modifying feeds if needed) and it will do almost nothing on these toolpaths. So I d say that Mastercam HST, even if they need to be improved in certain circumstances (mainly thin walls), are pretty reliable and consistent.    

[R. Van Winkle]

On 5/19/2017 at 0:47 PM, BenK said:

27% air cutting time is a lot.

That's what I'm saying! And like I said, when I walk by a machine and see it running volumill in stinkin' aluminum I get edgy.... throw a damned face mill in there and move that metal!

On 5/19/2017 at 3:29 PM, Jay Kramer @ Precision Programming said:

So you are not a Mastercam customer now?

I wonder if they have mad any improvements to the Volumill tool. it used to be an add-on for Mastercam at one time. Just like HSM paths from Autodesk started as a option for Mastercam.

No, not a customer now. We're using Gibbscam. (Yea, I know, don't rub it in meh face mkay?)

I'm sure they have. And I haven't touched MCam for years so I'm not up to speed with what they're up to. Hearing some, um, interesting(?) stories about 2017 and the ribbon bar. Lots of power users seem to be upset that they've been kicked to the curb in favor of book-smart kids that want something simple, not powerful. But I digress. I'm trying to convince the company to move away from Gibbscam. Been thinking about pushing towards Mastercam but will need to see if it's as bad as I've heard.

On 5/20/2017 at 1:53 AM, David Colin said:

To answer original question : Mastercam HST control tool engagement angle (as almost all dynamic toolpaths from any CAM). In Mastercam toolpaths parameters, you set a radial engagement but Mastercam will internally calculate equivalent engagement angle and will use that to generate its toolpaths (IMHO this info should be added in GUI).

Dynamics toolpathing goal is to maintain a constant hm value for each move during toolpaths. There is 2 main ways to achieve it: maintaining a constant tool engagement angle for every point in toolpaths or adjusting feed according to engagement angle.

I used Volumill a few years ago with MastercamX3 addon then with stand alone Nexion versiin but it's probably been greatly improved now. I d say Volumill 'mainly' use engagement angle to generate its toolpath (but not only) then adjust feed to maintain hm.

Mastercam is tool engagement all the way. This is why in tighter corners it almost generates spring passes as radius toolpath is near tool radius (perhaps it should lightly increase tool engagement angle and reduce feed in that circumstances? It s up to CNC to experiment and check what is more productive or will offer a better tool life). I still dislike the way it manages first pass on outer corners of a square stock (it seems to overload tool increasing radial engagement) but if you check it, you will see it maintains tool engagement angle. I also checked Mastercam dynamic toolpaths with Vericut Optipath, asking it to maintain chip thickness (modifying feeds if needed) and it will do almost nothing on these toolpaths. So I d say that Mastercam HST, even if they need to be improved in certain circumstances (mainly thin walls), are pretty reliable and consistent.    

Thanks David. I'll print this out and use it as a reference next week when the rep comes in.

[Guest]

17 minutes ago, R. Van Winkle said:

That's what I'm saying! And like I said, when I walk by a machine and see it running volumill in stinkin' aluminum I get edgy.... throw a damned face mill in there and move that metal!

A bit of an over generalization, no?

Where I work and it won't last long......a lot of aluminum but intricate work where a "Face Mill" isn't going to be much help

Edited May 21, 2017 by Guest

[R. Van Winkle]

12 minutes ago, JParis said:

A bit of an over generalization, no?

No.

[Guest]

1 minute ago, R. Van Winkle said:

No.

lol, ok

[civiceg]

Doesn't sound like a software problem.... 

[BenK]

54 minutes ago, R. Van Winkle said:

That's what I'm saying! And like I said, when I walk by a machine and see it running volumill in stinkin' aluminum I get edgy.... throw a damned face mill in there and move that metal!

To my point, its really how the programmer applies the path. The largest metal removal rate I have ever seen in aluminum was using a Dynamic path (Mastercams Volumill equivalent) and a 2.00" square shoulder mill. Saying you should never use it is like throwing the baby out with the bathwater.

[Newbeeee™]

1 hour ago, R. Van Winkle said:

 Hearing some, um, interesting(?) stories about 2017 and the ribbon bar. Lots of power users seem to be upset that they've been kicked to the curb in favor of book-smart kids that want something simple, not powerful. But I digress. I'm trying to convince the company to move away from Gibbscam. Been thinking about pushing towards Mastercam but will need to see if it's as bad as I've heard.

Have NOOOOOOOOOOOOOOOOOOOOOOOOOOOOOOOOOOOOOOOOOOOOO fear

Ribbon interface coming to GibbsCam on a 'puter near you soon!

[R. Van Winkle]

2 hours ago, civicegg said:

Doesn't sound like a software problem.... 

At this point it's not. It's an old garage shop mentality trying to join the 21st century. Volumill is their go-to path no matter what the geometry. Drives me bonkers. They're starting to see how much faster things can go but it's like pulling teeth. They just don't want to move out of their comfort zones.

1 hour ago, BenK said:

To my point, its really how the programmer applies the path. The largest metal removal rate I have ever seen in aluminum was using a Dynamic path (Mastercams Volumill equivalent) and a 2.00" square shoulder mill. Saying you should never use it is like throwing the baby out with the bathwater.

This. This! A thousand times this! And to your point, I didn't say they should never use it. They use it way too much when doing simple square outlines etc.

[R. Van Winkle]

1 hour ago, newbeeee said:

Have NOOOOOOOOOOOOOOOOOOOOOOOOOOOOOOOOOOOOOOOOOOOOO fear

Ribbon interface coming to GibbsCam on a 'puter near you soon!

Where's that damned unlike button...

[Newbeeee™]

1 hour ago, R. Van Winkle said:

Where's that damned unlike button...

Oh you'll HAVE to like it.

It's the future...

[R. Van Winkle]

57 minutes ago, newbeeee said:

Oh you'll HAVE to like it.

It's the future...

I suppose you're right. The software is getting smarter so people don't have to.

I need a nap.

[gcode]

5 hours ago, R. Van Winkle said:

Been thinking about pushing towards Mastercam but will need to see if it's as bad as I've heard.

I don't care for ribbon bar interfaces, but I have MC2017 customized to my liking, and wouldn't go back to X9 for lifetime free maintenance.

Of course if I went back to X9 I wouldn't need free maintenance.

The pluses out weigh the minus IMO

 

[Guest]

Yep, the GibbSCAM snobs wi be howling like the rest of us in no time.