Any way to speed up cutting?

[joewinslow]

Howdy Everybody -

Anyone have any software/hardware suggestions on speeding up cutting speeds? I'm finding myself with 10-15 hour cut times...

When I bumb up the speed, my PRT96 (2006) seems to start "skipping" and leaving very uniformly spaced pock-marks.

I cut alot of 2D - 3D work that requires a tremendous amount of travel in the Z range.

[Brady Watson]

Steve,
What model PRT is it? - A standard PRT, PRT 4th Generation (4G with Geckodrives) or PRT Alpha?

What software are you using to generate your 3D SBP files?

There are several things you can do depending on the machine & software used to speed up cutting.

-B

[sailfl]

Joe, you do very nice work. Being in Washington, DC you must get a lot of work.

[joewinslow]

Thanks Nils. I do get a fair bit indeed.

Brady - I'm using a PRT96 Alpha. Using VectorArt3D Machinist and VectorArt Cut 3D.

Call me "Joe".

Thanks!

[jhicks]

One thing to check based on your comment about Z travel is to control/syncronize the Z speed better in relationship with X & Y. Depending on cut depth and any roughing passes used or not, ( we generally avoid roughing passes and go entirely with the final ball nose starting on the highest surface usually the center and work out and down from there at full depth and small 8% to 10% step over) you can increase Z plunge and/or accelleration ramps so it isn't slowing down the x and y speed waiting for the Z. This may be the cause of the Jerkiness you describe.
If you are running at 180 IPM for example as the programmed move speed and have high safe Z plus slow plunge and soft ramp curve, you will never see the X or Y hit full speed between plunges because it never will have time to ramp up or down. You compound the accumulated impact if you have a high safe Z between moves when all you really want to do is clear the surface slightly and keep moving.
Lots of variables to be syncronized to optomize x,y, and Z speeds but I'm sure Brady will give you all the particulars when you discuss with him.
Those files must be some pretty large pieces to even approach that kind of time so post photos of the finals. I usually think about 3d times as approximately 30 to 60 minutes per square foot of area being machined as a mental guideline before tinkering if that helps.
How many lines of code is this file? Sometimes that will give you an idea of potential run time but only as very generalized a guideline.

[joewinslow]

Thanks Jerry, I appreciate the help. I use a ton of code - some are in the 300K lines plus.

I recall in the past hearing of some type of software that joins the code strings together - this, from what I understand - allows the processor to feed the machine one continuos movement command vice thousands of small movements. These small movements, computed at high speeds, are what I've heard produce the jerkiness and slow it down. I thought I heard this lopped off around 40% of the machining time... Ever heard of what I'm talking about?

Brady - any thoughts?

[Brady Watson]

Joe,
Let me start by saying that 3D 'takes as long as it takes' - and while you can make a few tweaks here and there to gain speed, they are often at the expense of finish quality.

I would encourage you to explore adjusting your ramping settings via the VR command - keeping in mind that ramps for a 3D file will be very different from a 2D file and will often need changing between 3D reliefs depending on the amount of detail in the relief.


4722

The areas highlighted in green show the ramp settings that most influence 3D ramping. The Move Ramp Rate has been set to 0.1 (hard to see decimal) and this will make cutting very aggressive. If you have a well tuned machine with no slop in it, then the cutting result will be very good, but the machine will sound like it is moving more harshly than if it was set to the default 0.2. This value reduces the amount of ramping - hence the harsher machine action. Be careful with this setting as it can cause the machine to go into Alpha mode if you have your speeds all whacked out...(see after SCS)

*Use the US and UR commands in SB3 to save your various configurations, and save them with a meaningful name. Use US to save a configuration and UR to call it up again.

The 3D Threshold value is at 100 by default, I've found that a value of 150 is good for most things. The function of 3D Thershold is to reduce the sensitivity of ramping when cutting 3D. Set this to 150 and leave it alone.

Minimum Distance to Check - set to .08, this value is inversely proportional to what you think it is. It checks for the smallest move that will trigger ramping. 0.08 is a good all around setting. Leave it at .08

Nothing influences 3D ramping more than Slow Corner Speed (SCS). I will run anywhere from 25 to 65 depending on how much detail is in the file. If you have a relief with a large stippled background, requiring the Z to move up and down a lot in short succession, then dial the SCS down a bit. This also holds true if your 3D file is meeting a flat wall at the end of each raster pass. Pull down the SCS to prevent banging. Play with this setting on your own to determine how to tune it for what you do. This setting, plus the Move Ramp Rate will help you to adjust how aggressively a file is cut. If the tool is 'banging' then reduce SCS or increase Move Ramp Rate.

Move Speeds - In general, you want your XY and Z speeds to be the SAME, depending on your tool. Naturally, you don't want to run the Z faster than 3 IPS, as it is hard (especially with a non-geared Alpha or 3.6 or 7.2 Standard tool) as it just can't catch up sometimes. I have found that 3,2 and 5,3 to be good speeds for 3D, providing that the relief is the appropriate size - USE YOUR BRAIN - If the relief to be cut is only 5" wide, then you are NOT going to cut it at 5 IPS...and if you throw speeds too fast at it, you will get jerky moves because SB3 is checking each move, the angle in which the tool moves (in XZ and YZ directions) and grades the ramping according to the angle that the tool needs to move - it gets complicated quickly - Just know to use common sense when setting speeds. Naturally, larger reliefs run faster than smaller reliefs - inch for inch - provided that there are not a bunch of tiny moves in the file that it needs to make - such as a background texture.

So in all reality - there is no 'one ramp fits all' recipe that I can give you. I tune ramps for every file so that they give me the best balance between speed and quality. I've run 3D files that take 30hrs to cut - if I could cut it faster I would, but it takes as long as it takes...

I know you are not running ArtCAM Pro, but for those that do, that want an instant increase in speed and machine smoothness, pull your tolerance setting in the 3D Relief Machining fill-in sheet from the default .0001 to .0025. It is doubtful that you will need a tolerance greater than this unless you are doing micromachining of 3D where the tolerance needs to be this fine. Your file size will also be reduced by a factor of 5 (50 meg file now 10 meg). It would be nice if Cut3D added a tolerance setting, but then again we could gone on for days about 'what would be nice' and what is reality.

-B

[joewinslow]

Brady - thanks for taking so much time on this - I greatly appreciate it.

I'll read it more in-depth this week and get back to you with the results.

Thanks amigo!
Joe

[Brady Watson]

No problem, Joe. People ask for advice on ramping...but this will need to get posted in my Tips & Tricks section or the Wiki (or both) in order for people to get the most out of it.

-B

[khalid]

Just read this of my technique for speeding up the 3D contouring... I cut 75% of time while implementing this technique..

http://www.vectric.com/forum/viewtopic.php?f=28&t=4220&start=0
http://www.cnczone.com/forums/showthread.php?t=68544
Best Regards
Khalid

[jeffreymcgrew]

One thing that made our 3D carving go way down in speed is better toolpathing via better software.

I don't know anything about the CAM you're using, so take this with a grain of salt. But when we went from using Ventric's Cut 3D, where you just raster everything out, to Ventric's Aspire, where you've got much better control and more options for the 3D toolpaths, well, our toolpath times dropped quite a bit because we could be smarter about the moves the machine made. I'm certain that Artcam or others (and maybe the CAM software you're using) has even more and better options, but I thought I'd throw this out as well.

[nick]

Well I think that alone can justify the cost of Aspire for 3D cutting...

Thanks alot for this post

[khalid]

Nick...Thanks a Lot for This Post??????????????????What one man ;)

[joe_winslow]

Thanks Jeffrey - I did download a trial version of aspire but have not had a chance to really run it yet. Ill let you all know how it goes.