Efficient roughing path

[lowcountrycamo]

I am programming a stack of parts for our new Makino mag1.  All are 7050 Al aero structure.  I have been thinking about most efficient path for roughing and finishing pockets and floors.  On the slower machines I use mostly zig zag as there is more straight moves and I like the pattern appearance for finishing. 
I was also considering ways to limit wall finish passes to 1 for walls.  
any comments or opinions?

thanks

steve austin

[Leon82]

I would use dynamic or pocket highspeed which ever is faster. I would try both high step over shallow cut and full depth light radial and see the time difference.

then a separate zigzag finish pocket at final depth to get your floor finish.

[JParis]

4 minutes ago, lowcountrycamo said:

I was also considering ways to limit wall finish passes to 1 for walls.  
any comments or opinions?

thanks

steve austin

That will be VERY much part & tolerance dependent.  I know when I have tight tolerances, I have to run multiple passes to consistently hold size.

Sight unseen, as parts can have different requirements & strategies, I'll talk in generalities.

I look at using a 3D Optirough becasue of the cutting paths....I remember the days of having to program cuts down and being limited but the geometry requirements. With Optirough, I can get into full depth cuts and then step up in areas that need to....that roughing path alone can be a huge time saver...With that cutting style, I tend to try to not use too many restmills to get corners down in size...but I will if the geometry supports it...

Use zones to work areas that may require a different approach. Yes, this mean geometry creating usually, surfaces and/or wireframe...

I like to look at all the paths when done, before posting and see which paths are the longest run time....I then evaluate those to see if I can change anything..

 

[crazy^millman]

It is very subjective to the part and the machines I have to program with. I will say I took an 100 hour roughing years ago using that zig zag for everything process out of NX and used Optirough and was able to rough in 40 hours. We will pulling 180 cubic inches a metal a minute.

[lowcountrycamo]

So I always thought optirough carried much wasted motion with a lot of accl/decell slippage.  For those not familiar this machine is 120kw/160 hp 33,000rpm  with tap testing.  We are cutting wing ribs, logerons, a frames.  Mostly thin walls and floors .05-.150”with pockets 1 -2” deep. I understand this is vague.  Thanks

For reference this is the type of parts we are running 

 

[JParis]

I look at that motion and in my opinion, WAY too slow

[lowcountrycamo]

1 hour ago, JParis said:

I look at that motion and in my opinion, WAY too slow

You mean federate or motion pattern?

[lowcountrycamo]

Are you guys using Dynamic and opti- rough paths for large aluminum parts?   I generally use them on ti and steel.  

[Leon82]

46 minutes ago, lowcountrycamo said:

Are you guys using Dynamic and opti- rough paths for large aluminum parts?   I generally use them on ti and steel.  

I do. Step up comes in handy when you deal with ribs

[cncappsjames]

On 12/3/2022 at 10:08 AM, lowcountrycamo said:

You mean federate or motion pattern?

Feed and motion. And yes, dynamic in Al. as well. I've found I can pull higher cubes AND get more consistent results. 

Long feed moves like that should be hitting close to 60m/min. in Al. with that kind of available HP. 

I'm with @JParis... work like that MAX DOC step up if necessary especially with ribs... generally speaking of course. I'll cut 7075 with different strategies than 7050, and different than 6061.

JM2CFWIW 

[Aaron Eberhard]

The other reason to default to Dynamic/Opti is that they generally put less stress into the part, if flatness or tolerances are tight on the finish product you'll get a lot less distortion when you unclamp than with traditional methods.  You can dial in the amount of load you're putting into the material, and often trade a bit of roughing time to not have to do a second "finishing" op after releasing/skimming/reclamping the part.    Sometimes it's not raw toolpath time that's the big win.

[lowcountrycamo]

So when the machine arrives, we'll takes some test cuts showing traditional vs dyn in 7050.   I have always understood dynamic as a more reliable path.  However, in some instances I have noticed a tremendous about of time slippage due to accel/decell on larger slower machines.   Having long thought about the most efficient patterns for roughing and finishing these large parts, I have searched out but found very little examples.   I very much appreciate your insight and experience.

steve austin

[Aaron Eberhard]

One thing to be careful of with the Opti/Dynamic toolpaths is to make sure your microlift distance and speed is more reasonable for a linear way modern machine.  There's no reason to back off .01" unless you've got a ton of Z axis backlash, .002-.003 should be fine.  Max out your back feed rate to whatever the machine can theoretically traverse at.  It defaults to 100IPM, which is way too slow, especially since you'll be aiming for >2000 IPM range most likely...

[gcode]

53 minutes ago, Aaron Eberhard said:

It defaults to 100IPM, which is way too slow, especially since you'll be aiming for >2000 IPM range most likely...

and you'll probably have to hold the operator's hand the for the first couple of programs

if you are not used to dynamic roughing on a machine capable of very fast feed motion F1000 or F2000 back feed motion

can be terrifying 

[heavychevy2155]

Don't be afraid to try 2d dynamic toolpaths with custom entry chains, just a simple line and some additional slot width can give a drastically different path.  

[Colin Gilchrist]

19 hours ago, Aaron Eberhard said:

One thing to be careful of with the Opti/Dynamic toolpaths is to make sure your microlift distance and speed is more reasonable for a linear way modern machine.  There's no reason to back off .01" unless you've got a ton of Z axis backlash, .002-.003 should be fine.  Max out your back feed rate to whatever the machine can theoretically traverse at.  It defaults to 100IPM, which is way too slow, especially since you'll be aiming for >2000 IPM range most likely...

This is where editing the Defaults File, and setting up a Defaults File > for each machine, where you edit the File Extension from '.mcam-defaults' > to '.mcam', then open the file inside Mastercam, you can then replace the "Default machine" in the Machine Group Properties, with your actual machine. This gives you the same coolant/drilling/misc value strings, available in the Defaults File. Then, just go through the Default Operations, and set all your desired starting values for the various toolpaths, especially Dynamic and Opti-Rough.

So, as an example, if you had machines with different Accel/Decel parameters, and wanted your older machines to have a 350 IPM Backfeed, and the more advanced machines to use 875 IPM, you'd just setup different Operation Defaults Files. The Operation Default Files can be associated back to a Control Definition File, (Under the Files page), which means you can have different programming default options, when you use different Machine Definitions (and associated CD Files > pointing to customized Operation Default Files).

Just be sure to edit both the actual name of the 'Mill_Inch.mcam-defaults', (make a copy first, then change the file name), then edit the file extension, open as a Mastercam File, then 'replace the machine definition inside this File, edit your Op defaults, (For example, I enable Coolant/After, turn on the Filter on all my operation types, and turn on things like Misc. Values to enable High-Speed output), and save the file. Finally, you need to go back to the Ops Folder, and modify the File Extension from '.mcam', back to '.mcam-defaults'.

[Colin Gilchrist]

20 hours ago, Aaron Eberhard said:

One thing to be careful of with the Opti/Dynamic toolpaths is to make sure your microlift distance and speed is more reasonable for a linear way modern machine.  There's no reason to back off .01" unless you've got a ton of Z axis backlash, .002-.003 should be fine.  Max out your back feed rate to whatever the machine can theoretically traverse at.  It defaults to 100IPM, which is way too slow, especially since you'll be aiming for >2000 IPM range most likely...

By the way man, I loved "The Perfectionists"! Finally made the time to read through the last few chapters. I love his writing style, and the content. Great book. We should get together for lunch soon so I can return it to you. 

[Aaron Eberhard]

3 hours ago, Colin Gilchrist said:

By the way man, I loved "The Perfectionists"! Finally made the time to read through the last few chapters. I love his writing style, and the content. Great book. We should get together for lunch soon so I can return it to you. 

Glad to hear you liked it. I really enjoyed it too, it was like sitting with an old friend discussing and learning

Absolutely, let's figure out a time in the next few weeks!

[gms1]

On 12/3/2022 at 12:08 PM, lowcountrycamo said:

You mean federate or motion pattern?

 

I look at that toolpath as a little inefficient and unbalanced. I see ramps into material which is nice but not needed when you can enter off the end of the part. The path that comes back to the left side of the part after it runs the different rib shapes has all kinds of different material engagement percentages so you couldn't really speed that cut up because you might be 10% tool diameter engaged then 2 seconds later 60% engaged. Your tool loads are gonna be all over the map with that toolpath.

This might not mean much depending on what you are after to make the money. There are times I will climb/convention mill pockets just cause I want it done right noooow. and I don't care about tool life because I have 3 more bodies sitting in reserve ready to drop in when the tool changes. If I am trying for tool life and doing long runs, ya I might tighten up some parameters and manage the engagement of the tool which may make more money in the long run for big production job.