Best Cam from a processing speed standpoint?

[mhajicek]

One "gotcha" to watch out for in Mastercam is the memory settings. By default it's set to use I think only 40% or 50% of your RAM. Set it to 80% (and have a lot in your computer) and you'll do much better on large paths.

When it runs out of RAM it starts paging to disk, and calculation time increases exponentially. At a previous job years ago, I had to break operations up to keep the working memory for each under the RAM limit.

 

[boosted]

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

That's a cool part, but not that CAM intensive from what I can see. It's just top down. Not really a great example of something that should take forever to crunch.

Several times a year I post parts that are in the 250MB+ range. Sometimes they take all night to calculate in hyperMILL. Things like "tilt to avoid" are extremely processing intensive. Porting with a lollipop, or finishing obscured surfaces where it has to constantly change the angle - those are things that kill processing time.

Years ago I tried WorkNC for a month, and really liked it. I bet it could beat hyperMILL from a raw processing speed standpoint. I rarely find processing speed to be an issue though. Especially since hyperMILL lets you continue to work while it crunches in the background.

 

[Marvel]

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.

I don't, I tried it a while back but never noticed much of a difference.

 

[boosted]

Here's a couple pictures of the kind of thing I would call really processing intensive. Calculating all of the undercuts for the inside of the part (approximately 17in long) took about 9 hours. That is excessive, but it is all five axis rework, and must find tilt solutions and change tangency so it can squeeze a 9.5in long holder and tool assembly inside the cavity without smacking the spindle face on the part or stock.

 

[Marvel]

That's a cool part, but not that CAM intensive from what I can see. It's just top down. Not really a great example of something that should take forever to crunch.

Several times a year I post parts that are in the 250MB+ range. Sometimes they take all night to calculate in hyperMILL. Things like "tilt to avoid" are extremely processing intensive. Porting with a lollipop, or finishing obscured surfaces where it has to constantly change the angle - those are things that kill processing time.

Years ago I tried WorkNC for a month, and really liked it. I bet it could beat hyperMILL from a raw processing speed standpoint. I rarely find processing speed to be an issue though. Especially since hyperMILL lets you continue to work while it crunches in the background.

It wasn't meant to be an example of something that "should take forever to crunch" and nowhere did I say it was "CAM intensive". You must not have read the post I replied to, the part I shared was relevant in comparison to BlushInventors post about his experience with CAMWorks calculating and generating a Volumil tool path that took over night.

 

[Matt_W]

Several times a year I post parts that are in the 250MB+ range. Sometimes they take all night to calculate in hyperMILL. Things like "tilt to avoid" are extremely processing intensive. Porting with a lollipop, or finishing obscured surfaces where it has to constantly change the angle - those are things that kill processing time.

You might know this, but a tip I was give was given during my training was to try keep the angle to a minimum in the max range field in the collision avoidance section. When it is calculating the toolpath and it sees it is in collision it will try calculate the path with the max angle for avoidance first, then if it sees it out of collision with will calculate again at a reduced angle and so on until it can find the smallest angle that will keep it out of a crunch. So the max angle is a large one, then it has a lot more work to do.

I always try and use manual curve rather than automatic avoidance, where I can. Automatic can in general take some calculating.

 

[Matt_W]

That sounds along time? are you using with a manual curve? without fully looking at it, to me only the corner undercut would I think may have to use the collision avoidance with a drive curve in the correct position.

 

[boosted]

You might know this, but a tip I was give was given during my training was to try keep the angle to a minimum in the max range field in the collision avoidance section. When it is calculating the toolpath and it sees it is in collision it will try calculate the path with the max angle for avoidance first, then if it sees it out of collision with will calculate again at a reduced angle and so on until it can find the smallest angle that will keep it out of a crunch. So the max angle is a large one, then it has a lot more work to do.

I always try and use manual curve rather than automatic avoidance, where I can. Automatic can in general take some calculating.

I don't know all the tricks, but I know a lot of them. Sometimes things just take forever to calculate. I often forget that parts which are physically larger take longer too. Rework is a killer. Even with all the tricks turned on, rework sometimes takes forever. One of my few major complaints about hyperMILL is that if one path fails when crunching overnight it doesn't move on to the next one. Nothing worse than coming back to a stack of uncalculated toolpaths because you forgot to set the clearance plane on a chamfer operation.

Anyways, I would love to run a side-by-side on some really ugly five axis paths just to see which CAM software was the fastest. I bet one of the more "obscure" systems like Tebis blows everything else away. Somebody at a tech company that has every CAM system under the sun should setup a comparison.

 

[BluishInventor]

Anyone have a part they can upload or link to that would cause several minutes of calc time? Folks could then benchmark their system/setup and post their parameter settings, computer specs, and calc time results. Some might even learn a thing or two from more advanced users. Or start a war. Who knows?

 

[BRIAN.T]

Anyone have a part they can upload or link to that would cause several minutes of calc time? Folks could then benchmark their system/setup and post their parameter settings, computer specs, and calc time results. Some might even learn a thing or two from more advanced users. Or start a war. Who knows?

Mastercam has a standard benchmark file they use for this. If you're a mastercam user reach out to your reseller. I might have it somewhere too.

 

[BRIAN.T]

One "gotcha" to watch out for in Mastercam is the memory settings. By default it's set to use I think only 40% or 50% of your RAM. Set it to 80% (and have a lot in your computer) and you'll do much better on large paths.

When it runs out of RAM it starts paging to disk, and calculation time increases exponentially. At a previous job years ago, I had to break operations up to keep the working memory for each under the RAM limit.

Excellent! I'm testing now. It was set to 50 percent.

 

[BluishInventor]

Mastercam has a standard benchmark file they use for this. If you're a mastercam user reach out to your reseller. I might have it somewhere too.

I don't have MC. But I think it would be cool to come up with a benchmark that could be used with any CAM system.

 

[Matt_W]

I don't have MC. But I think it would be cool to come up with a benchmark that could be used with any CAM system.

That would be a good idea!

 

[BluishInventor]

Ok, here is the start of something. The goal of this part would be to have a cube with different features on each side. Each feature would test a different type of toolpath.

This first side would test Volumetric/Dynamic Roughing toolpath calculations. Obviously, each CAM system will have different parameters, so we will need to figure out how to best setup these parameters so that each system can be spec'd to be the same.

Tool:
0.2500 x 1.250LOC 4FL Endmill 2.500 OAL (no holder)

Stock:
Bounding box of model. No excess.

Volumetric/Dynamic/HSM Rough Operation Parameters:
10% Stepover
0.250 Step Down (no intermediate steps)
0.010 Stock to leave in XYZ
5% Minimum tool path radius (percent of tool dia)
1.000 Clearance Plane
Machine from existing stock
Collision Detection ON
0.002 Machining Tolerance/Deviation (facet size, this can be increased to lengthen calc times)

Couldn't post a photo for all my settings(limited to 5). I imagine it will take a bit of discussion to come up with operation parameters that everyone can use. This is just a start.

To post your results, I would say one should get a snippet of All operation parameters, toolpath image, image of calculation time, and computer specs(OS, CPU, GPU, RAM, etc).

Let me know your thoughts. And if you have an idea for another tool path type/geometry addition to the model that is calculation intensive, Post it!

If a baseline can be built, then maybe we can start a Sticky Thread in CAD/CAM with full instructions/files and everyone can share their results.



Sorry if the photos are shite quality, not sure why that is.
View attachment Benchmark.zip

 

[BluishInventor]

Part and Toolpath

 

[5 axis Fidia guy]

That would be interesting for someone to post a model and set some parameters for guys to try with their system and see how it does. I'm a long time Powermill user, almost 30 years worth. I really have nothing to compare it to, but I'm very impatient and it always seems to take too long. I just finished up a project with a mold core and it had over 100 toolpaths, along with that several models, and boundaries and all the goodies that come with it. Most of my finishing tolerances are .0001 inches with many simultanious toolpaths, and things take a while, especially while collision checking. Powermill is multi threading on some things, but not all, they do however have the option to queue toolpaths so you can just keep on working. I usually batch big toolpaths and run the calculations overnite if possible. In my situation, the outcome of the SAFE toolpath is more important than flat out speed, since not much progress is getting done with a smashed spindle.