Best Cam from a processing speed standpoint?

I'm running mastercam, and I like it. We ran mastercam's benchmark test and got the fastest speed of anyone who tried (at the time) maybe a year ago. We've got a really good computer. Unfortunately mastercam is limited to single core processing for most things.

I hate waiting 10 minutes for some of these intense multi axis paths.

What high end cad/cam system has the best processing speed?

Mastercam is not always limited to single core. It will use multiple cores quite often. It will even use the video card for crunching numbers in some instances.

This single core thinking comes from the fact that some toolpaths need to calculate step 1 and 2 before it has enough information to calculate step 3. This type of process is limited to a single, linear calculation using a single core. Every software crunching this type of process will be roughly the same in processing time. That's why we tend to focus on CPU speed over everything else.

What CPU are you using now? The 12th gen i9 are setting impressive times.

Without knowing your workflow, as a suggestion, set your tolerances and stepovers loose until you have the motion you want, then tighten things up. Should avoid long wait times when getting things dialed in.

mike_w said:

Mastercam is not always limited to single core. It will use multiple cores quite often. It will even use the video card for crunching numbers is some instances.

This single core thinking comes from the fact that some toolpaths need to calculate step 1 and 2 before it has enough information to calculate step 3. This type of process is limited to a single, linear calculation using a single core. Every software crunching this type of process will be roughly the same in processing time. That's why we tend to focus on CPU speed over everything else.

What CPU are you using now? The 12th gen i9 are setting impressive times.

Without knowing your workflow, as a suggestion, set your tolerances and stepovers loose until you have the motion you want, then tighten things up. Should avoid long wait times when getting things dialed in.

Click to expand...

That's interesting, I wasn't aware of that. But that does make me feel better.

As for setting things loose, I always do that. The problem (as I'm sure you know) is most times I need the final toolpath/stock model in order to move on, not necessarily the toolpath by itself.

mike_w said:

Mastercam is not always limited to single core. It will use multiple cores quite often. It will even use the video card for crunching numbers in some instances.

This single core thinking comes from the fact that some toolpaths need to calculate step 1 and 2 before it has enough information to calculate step 3. This type of process is limited to a single, linear calculation using a single core. Every software crunching this type of process will be roughly the same in processing time. That's why we tend to focus on CPU speed over everything else.

What CPU are you using now? The 12th gen i9 are setting impressive times.

Without knowing your workflow, as a suggestion, set your tolerances and stepovers loose until you have the motion you want, then tighten things up. Should avoid long wait times when getting things dialed in.

Click to expand...

It's something of a fallacy that multiaxis toolpaths are inherently linear, but there are large differences in the technical challenges required to make it work between different types of toolpaths.

Z level/waterline paths for example are trivial to parallelise - one thread to calculate the scanline instances, which can then spawn as many worker threads as it wants and let them calculate x number of scanlines, then a single thread pass at the end to calculate the link moves.

Parallel/raster toolpaths the same.

Toolpaths that are not pattern based present much more of a challenge to divide. Knowing where to start one segment being calculated in a discrete thread is impossible if you haven't yet calculated where the previous segment stopped, so some kind of workarounds are required if you want to divide those paths.

A potential method for example might be to parallel calculate sections of the toolpath that don't meet where they start and end, and follow up with a second pass to fill in the gaps - depending on the toolpath type this might be trivial or complicated, for a 5 axis swarf/trim type toolpath for example, this might be fairly simple to do, but would likely require a third pass to blend rapid changes in the tool axis that might occur in the fill-in segments etc.

Doing this with pseudo pattern based projected toolpaths would be more complicated as the fill-in segments would have to morph between non-uniformly placed points to maintain some semblance of the pattern.

TLDR: more difficult conversions to parallel computing have been successfully implemented in other disciplines of computing, and I do think that this is very underdeveloped in the CAM world.

BRIAN.T said:

What high end cad/cam system has the best processing speed?

Click to expand...

I can't answer that part, but don't most of them use Moduleworks toolpaths? So wouldn't the processing time be relatively similar?

Sorry if this is captain obvious, but you have this enabled?

Mtndew said:

I can't answer that part, but don't most of them use Moduleworks toolpaths? So wouldn't the processing time be relatively similar?

Click to expand...

Again not directly answering OP's question, but likely yes all systems using MW toolpaths are probably much the same.

It would be interesting to have a definitive list of non-MW systems.

PowerMill
HyperMill
WorkNC?
..
..
NX has MW integration, but I'm not sure to what extent as they have plenty of native toolpaths prior to MW.

WorkNC appears to have options for using up to 24 cores, although it appears to be primarily parallel processing of multiple toolpaths, as opposed to parallelisation of a single toolpath.

Mike1974 said:

Sorry if this is captain obvious, but you have this enabled?

View attachment 347014

Click to expand...

Hmmm... Allow me to check. This could be very helpful.

Mtndew said:

I can't answer that part, but don't most of them use Moduleworks toolpaths? So wouldn't the processing time be relatively similar?

Click to expand...

I was thinking the same. Side note, Ive always heard hypermill is amazing, but they use MW, so I can't imagine it's THAT much more advanced.

gregormarwick said:

Again not directly answering OP's question, but likely yes all systems using MW toolpaths are probably much the same.

It would be interesting to have a definitive list of non-MW systems.

PowerMill
HyperMill
WorkNC?
..
..
NX has MW integration, but I'm not sure to what extent as they have plenty of native toolpaths prior to MW.

WorkNC appears to have options for using up to 24 cores, although it appears to be primarily parallel processing of multiple toolpaths, as opposed to parallelisation of a single toolpath.

Click to expand...

Man, you're an impressive dude. Thanks for these detailed answers! What system do you use?

BRIAN.T said:

I'm running mastercam, and I like it. We ran mastercam's benchmark test and got the fastest speed of anyone who tried (at the time) maybe a year ago. We've got a really good computer. Unfortunately mastercam is limited to single core processing for most things.

I hate waiting 10 minutes for some of these intense multi axis paths.

What high end cad/cam system has the best processing speed?

Click to expand...

I'm using CAMWorks and have programmed some intense multi axis paths and I think the longest it's ever taken to generate a tool path was maybe 2-3 minutes. That includes any multiaxis tool path recognizing previous stock removal or from a STL WIP file, including fixture (vise, clamp, etc) avoidance, tool holder avoidance and/or avoid areas enabled as well.

There's been a couple times a part with a lot of multi axis paths has came back and my stock comes in at a different size and I've had to update my stock and regenerate every tool path and even then, maybe 5-6 minutes to regenerate.


Processor: Intel(R) Core(TM) i7-5820K CPU @ 3.30GHz 3.30 GHz
Installed RAM: 128GB
Graphics: Radeon RX 480 8GB

I wouldn’t say one software is going to process tool paths faster than the next, I think it’s more based on your computers hardware and settings. I’ve worked at shops that had workstation computers for CAM that were terribly slow.

BRIAN.T said:

I was thinking the same. Side note, Ive always heard hypermill is amazing, but they use MW, so I can't imagine it's THAT much more advanced.

Click to expand...

From my understanding, Hypermill does not use MW. They do, however, license and use Volumill.

My experience with Camworks is much different than Marvel's. I had a super feature heavy part that drove me insane due to calculation times taking forever when roughing with Volumill. If you watch the message window, it would generate a faceted model(STL) of the part body for every toolpath which is not ideal. Obviously, if your toolpath accuracy is set high, time will increase dramatically. But the faceting stage, whether or not it is apparent to the user, does happen which is how they can calculate toolpaths in the first place. 3D printer Slicing software use STLs natively for this very reason; calculating toolpaths.

Another part we had that was super tiny, but relatively simple in geometry, took overnight to calculate a volumill path in camworks. I used this part, among others, when I did a CAM evaluation to see if it was worth changing systems entirely. Mastercam was about ~40 mins, Hypermill was about ~10 min, and CamTool was ~1 min. All using the CAM system's respective volumill/dynamic roughing. Same ae/ap, tool info, toolpath resolution, etc..

While MW does make a toolpath just fine, the implementation of it does matter.

I'm super happy that Marvel has had great results. We never did.

And as others have pointed out, while having a decent computer does speed things up, the linear processing of 1 path before the next will probably the norm until a new technology comes to fruition.

just my2c

I've been using CAMworks pro for years and recently started with SolidCAM. I can tell you on huge 3x (40"x50"x20")surfaces SolidCAM is much faster although both use muti-core processing with simultaneous threads. We generate 60MB gcode files one example took about 12minutes on CAMworks, same part was less then 5 on Solidcam. Can't really compare anyone else's stuff.

BOB-OO said:

I've been using CAMworks pro for years and recently started with SolidCAM. I can tell you on huge 3x (40"x50"x20")surfaces SolidCAM is much faster although both use muti-core processing with simultaneous threads. We generate 60MB gcode files one example took about 12minutes on CAMworks, same part was less then 5 on Solidcam. Can't really compare anyone else's stuff.

Click to expand...

I'd be interested it trying someone's CAMWorks file that took an extended period of time to generate toolpaths to see how much difference a computer can actually make.

I've read numerous times people complaining about tool path generating time taking too long, but like I said above, with my computer I am using now, that I built, I have never experienced anything that I felt was "too long". I did occasionally at previous employment with workstation computers and at one place they gave me a laptop that was ridiculous.

BluishInventor said:

From my understanding, Hypermill does not use MW. They do, however, license and use Volumill.

My experience with Camworks is much different than Marvel's. I had a super feature heavy part that drove me insane due to calculation times taking forever when roughing with Volumill. If you watch the message window, it would generate a faceted model(STL) of the part body for every toolpath which is not ideal. Obviously, if your toolpath accuracy is set high, time will increase dramatically. But the faceting stage, whether or not it is apparent to the user, does happen which is how they can calculate toolpaths in the first place. 3D printer Slicing software use STLs natively for this very reason; calculating toolpaths.

Another part we had that was super tiny, but relatively simple in geometry, took overnight to calculate a volumill path in camworks. I used this part, among others, when I did a CAM evaluation to see if it was worth changing systems entirely. Mastercam was about ~40 mins, Hypermill was about ~10 min, and CamTool was ~1 min. All using the CAM system's respective volumill/dynamic roughing. Same ae/ap, tool info, toolpath resolution, etc..

While MW does make a toolpath just fine, the implementation of it does matter.

I'm super happy that Marvel has had great results. We never did.

And as others have pointed out, while having a decent computer does speed things up, the linear processing of 1 path before the next will probably the norm until a new technology comes to fruition.

just my2c

Click to expand...

Overnight to calculate a tool path? That's crazy!

The images attached, this part is approximately 6" x 8" x 26" and I used a 3 Axis Volumil Area Clearance with a max DOC of 1.5" and .1" Finish/Rough Depth with .150 RDOC with quite a few surfacing finish paths that were programmed with .005" step overs. I counted 43 separate Multiaxis (surfacing) tool paths in the fist operation, and if I regenerate the full first OP tool paths it takes 6 minutes to regenerate everything. This first operations 3 Axis Volumil Area Clearance toolpath also has fixture and tool holder avoidance parameters and some avoid areas as well being used, it comes out to a 16MB NC file.

Marvel said:

Overnight to calculate a tool path? That's crazy!

Click to expand...

Yeah, it was pretty bad.

Not a bad looking part you got there. I take it that's a Haas?

BluishInventor said:

Yeah, it was pretty bad.

Not a bad looking part you got there. I take it that's a Haas?

Click to expand...

Yup, a VF3 SS

Marvel said:

Yup, a VF3 SS

Click to expand...

Curious and off topic; do you use CW to control your G187(Rough, Medium, Finish setting) with the Mach Deviation parameter? The post we had neglected to utilize that.

BRIAN.T said:

I was thinking the same. Side note, Ive always heard hypermill is amazing, but they use MW, so I can't imagine it's THAT much more advanced.

Click to expand...

I am 99.9999% sure that HyperMill doesn't use Module works , that the reason I moved to it.

I use HyperMill with an I09-10885, and its pretty quick compared to what I used to run it 10 years ago . Depends what you are trying to do and what 5 axis work you are doing. Difficult to say how it compare with the other without comparing like for like. If you post a part with an idea of a toolpath that's needed I can throw something at it and see what it gives.

I find it's like waiting for a kettle to boil, when it doesn't matter, you're not watching it and there's no rush, it calculates in a blink, but sitting there watching it desperate for the toolpath to get the job up and running its painfully slow.

Marvel said:

Overnight to calculate a tool path? That's crazy!

The images attached, this part is approximately 6" x 8" x 26" and I used a 3 Axis Volumil Area Clearance with a max DOC of 1.5" and .1" Finish/Rough Depth with .150 RDOC with quite a few surfacing finish paths that were programmed with .005" step overs. I counted 43 separate Multiaxis (surfacing) tool paths in the fist operation, and if I regenerate the full first OP tool paths it takes 6 minutes to regenerate everything. This first operations 3 Axis Volumil Area Clearance toolpath also has fixture and tool holder avoidance parameters and some avoid areas as well being used, it comes out to a 16MB NC file.

View attachment 347042
View attachment 347043
View attachment 347044
View attachment 347045

Click to expand...

Looks a nice job that, great work