Mastercam Optirough Stepup Parameters

[dodgin]

Bejesus - I remember that demo years ago. Rick is also known as Iscar Rick and did a bunch of videos many years ago. So he is an AE and not a salesman, but for Iscar and not MasterCAM.

Of course, right after I call Goose out for being a miserable cynic... this comes along and turns ME into a miserable cynic

I was always impressed by thinking OptiRough was actually this good!

Hold on...an Iscar guy not knowing what the FUCK he's talking about? Unheard of.

 

[gkoenig]

LoL - it is an awesome path though - if driven from a stock model it is just that much better and the fact that it can rough 90+% of a part in minutes very efficiently, is errr awesome! (I know I said that twice but it is )
It's just the finishing detail of a part, which takes the time.....!

Yes, but is it more awesome than HSM Works/Fusion Adaptive Clearing, NX Adaptive/3+2/5 Axis roughing? SolidCam iMachining? Volumill? Esprit Profit Milling?

Everyone is doing the stock-aware, HEM based algorithms now...

The problem is, I don't think anyone has ever done a straight-up comparison between all the available packages to see if there are any significant differences, advantages, or big disadvantages between any of them. They all make the same bullshit claims that they are the "Fastest" to machine stuff, but the comparisons are always against outdated roughing methods anyone who is concerned about making money stopped using as soon as they could.

 

[mhajicek]

LoL - it is an awesome path though - if driven from a stock model it is just that much better and the fact that it can rough 90+% of a part in minutes very efficiently, is errr awesome! (I know I said that twice but it is )
It's just the finishing detail of a part, which takes the time.....!

I've also used it for finishing mold cavity details. Semifinished with a .032" ball leaving .004", then Stock Model, then OptiRough using the stock model and a .020" ball. That way it takes extra passes and makes trochoidal loops where there's too much stock in the corners for a single pass. Finish was very good.

 

[mhajicek]

The problem is, I don't think anyone has ever done a straight-up comparison between all the available packages to see if there are any significant differences

That would be a tall ask. Who can afford to have all those software packages? Maybe if enough different shops got together, and all program the same thing to run on one machine for the test...

 

[gkoenig]

That would be a tall ask. Who can afford to have all those software packages? Maybe if enough different shops got together, and all program the same thing to run on one machine for the test...

Well, I've got 2/6. MasterCAM is easy to find someone to play ball. I know a few Esprit users. SolidCAM with iMachining and Volumill are the tough ones for me to find.

I will say, being curious about this - looked up iMachining again and boy... either their AEs don't know how to program a demo or iMachining is super unimpressive, but the time wasted was just massive.

 

[Marvel]

That would be a tall ask. Who can afford to have all those software packages? Maybe if enough different shops got together, and all program the same thing to run on one machine for the test...

Well, I've got 2/6. MasterCAM is easy to find someone to play ball. I know a few Esprit users. SolidCAM with iMachining and Volumill are the tough ones for me to find.

I will say, being curious about this - looked up iMachining again and boy... either their AEs don't know how to program a demo or iMachining is super unimpressive, but the time wasted was just massive.

I have CAMWorks with VoluMill.

Who is going to provide a file with parameters to follow? Don't necessarily need to run each program in a machine, could share the PGM files, and one could lay them out in a back plotter side by side for tool path comparison to see how close they are.

 

[goooose]

Direct comparisons can be difficult. What constitutes 'best'? Can one shape really give a good look into all these different toolpaths and their strengths and weaknesses? Would you purchase one of these softwares because their toolpath was 'better'?

As an example, some of these toolpaths are able to adjust the feedrate up or down depending on an internal/external arcing motion to maintain chipload. On a pocket type feature, this would theoretically hurt a toolpath capable of this feed override if comparing cycle times against a toolpath not capable of this. (feedrates need to be slowed down on internal arcs to maintain chipload)

Of the three I've used, I would pick Esprits Profit Milling just from an overall point of view of the resulting code on the majority of parts.
However, there are definite times I would rather use OptiRough or even Dynamic Mill just for ease of toolpath creation, knowing the resulting code would be similar from others. All things being equal or close to equal, ease of use of the interface is king.

 

[Marvel]

Direct comparisons can be difficult. What constitutes 'best'? Can one shape really give a good look into all these different toolpaths and their strengths and weaknesses? Would you purchase one of these softwares because their toolpath was 'better'?

As an example, some of these toolpaths are able to adjust the feedrate up or down depending on an internal/external arcing motion to maintain chipload. On a pocket type feature, this would theoretically hurt a toolpath capable of this feed override if comparing cycle times against a toolpath not capable of this. (feedrates need to be slowed down on internal arcs to maintain chipload)

Of the three I've used, I would pick Esprits Profit Milling just from an overall point of view of the resulting code on the majority of parts.
However, there are definite times I would rather use OptiRough or even Dynamic Mill just for ease of toolpath creation, knowing the resulting code would be similar from others. All things being equal or close to equal, ease of use of the interface is king.

I'd agree, I don't believe one could be defined 'best' based on toolpath alone. I'd be more curious how much the tool paths differentiate, if at all, with the same settings and then from there the ease of creating the tool path.

I know in CAMWorks for me, say to create a part perimeter and use Volumill, I can have that tool path created in 10 seconds with maybe 5 mouse clicks. Go to a 3 Axis VoluMill path, its maybe 15 seconds with a couple more mouse clicks. That's based on my default settings I use for 99% of my VoluMill toolpaths already being there.

 

[empower]

Yes, but is it more awesome than HSM Works/Fusion Adaptive Clearing, NX Adaptive/3+2/5 Axis roughing? SolidCam iMachining? Volumill? Esprit Profit Milling?

Everyone is doing the stock-aware, HEM based algorithms now...

The problem is, I don't think anyone has ever done a straight-up comparison between all the available packages to see if there are any significant differences, advantages, or big disadvantages between any of them. They all make the same bullshit claims that they are the "Fastest" to machine stuff, but the comparisons are always against outdated roughing methods anyone who is concerned about making money stopped using as soon as they could.

what would be a good demo to set up? i dont have much going on at work these days and could possibly do something.
i have NX, fusion hypermill and mastercam available to me. could easily do the same part/parameters on the same machine etc.
if we can put together a list of 'rules' to follow, i'd be down.

 

[Mtndew]

All things being equal or close to equal, ease of use of the interface is king.

I'd go one step further and say that having the option to make the interface how you like it is even better.
Meaning setting up your default icons and tabs so that your least used things aren't in the way.
That's how I have my Mastercam set up. I have 2 tabs of things that can do 99% of what I need.

 

[Marvel]

I'd go one step further and say that having the option to make the interface how you like it is even better.
Meaning setting up your default icons and tabs so that your least used things aren't in the way.
That's how I have my Mastercam set up. I have 2 tabs of things that can do 99% of what I need.

Agree, I have the same in CAMWorks, two tabs, I have a tab that's CAD buttons and the other is CAM icons/buttons. Eliminated all the icons that I never use.

 

[gkoenig]

i have NX, fusion hypermill and mastercam available to me.

What is the story with Hypermill's HSM/Roughing/HEM strategy? Are they licensing it or did they roll their own?

 

[empower]

What is the story with Hypermill's HSM/Roughing/HEM strategy? Are they licensing it or did they roll their own?

still volumill. i hear they're working on their own kernel but i dont think its quite ready yet.

 

[Marvel]

I created a part if anyone wants to use it.

I'm using CAMWorks with VoluMill and programmed a 3 Axis VoluMill Tool Path

Setup/Settings

Stock 2.75" x 6.25" x 6.25"
- Offset stock, left .01" on top

1/2" Endmill

12K RPM
150 IPM
.200 RDOC

Max ADOC - 1.5"
Cut Amount - .100"
Clearance - .01"

VoluMill
Entry Method - Spiral
Ramp Angle - 2 Deg
Entry Length - .100"
Floor Clearance - .01"
Smoothing Radius - 5%
Side Mill Only

CAMWorks Estimated Machine Time - 3.044
Actual Machine Time - 3:00 (Ran PGM cutting air)



View attachment Test Part.zip

 

[BugRobotics]

CAMWorks beats HSMWorks by about 17 seconds in estimated time.

HSMWorks estimated time: 3:22



EDIT: If I enable "both ways" adaptive and limit retractions I can get it down to 3:04.

 

[Marvel]

CAMWorks beats HSMWorks by about 17 seconds in estimated time.

HSMWorks estimated time: 3:22

View attachment 349235

EDIT: If I enable "both ways" adaptive and limit retractions I can get it down to 3:04.

View attachment 349236

If I enable both ways it drops it down to 2.85 (2:51)

I tried both ways once, when they first released it and didn't like it at all

 

[goooose]

As I mentioned earlier, this comparison is not going to reveal much as different toolpaths (patented algorithms) have different features, and of course the interface and options that the toolpath has available.

eg. in Mastercam using the above parameters, without me controlling the rest of the toolpath 3:20
if I start editing the microlift feeds, keep down limits, and retract control, I'm down to 2:30 (not using 'both ways')
I'm sure I could fiddle out another 10 seconds if I get into other optimizations.

 

[Marvel]

As I mentioned earlier, this comparison is not going to reveal much as different toolpaths (patented algorithms) have different features, and of course the interface and options that the toolpath has available.

eg. in Mastercam using the above parameters, without me controlling the rest of the toolpath 3:20
if I start editing the microlift feeds, keep down limits, and retract control, I'm down to 2:30 (not using 'both ways')
I'm sure I could fiddle out another 10 seconds if I get into other optimizations.

I think that's all quite obvious, but I think it was more a comparison to see how each systems creates the tool path on the same part to see how much they differentiate.

Toolpath time is somewhat irrelevant, because again obviously there are numerous settings that can be adjusted to shave time off, I more shared it along with actual machine time as a comparison to see how accurate CAMWorks calculation is with my machine settings within CAMWorks and real machine time.

 

[goooose]

I think that's all quite obvious, but I think it was more a comparison to see how each systems creates the tool path on the same part to see how much they differentiate.

Toolpath time is somewhat irrelevant, because again obviously there are numerous settings that can be adjusted to shave time off, I more shared it along with actual machine time as a comparison to see how accurate CAMWorks calculation is with my machine settings within CAMWorks and real machine time.

So were testing the cycle time estimation of the software then?? I'm confused

 

[Marvel]

So were testing the cycle time estimation of the software then?? I'm confused

Where did I say that? Maybe scroll up again and read.