Seek and Feed rates, depth passes

Talk about all things CNC
Post Reply
monkey123
Posts: 35
Joined: Sun Sep 08, 2013 3:36 am

Seek and Feed rates, depth passes

Post by monkey123 » Sat Nov 23, 2013 7:34 pm

I'm just getting my shapeoko underway. It has a table size of about 40x24" with a Z clearance of 6-8". DW660 cutting tool, Dual Y drive, Dual X makerslide, aluminum spacers throughout, and new motor mounts, etc. Using high current DRV8825 drivers that are heatsink and fan cooled. Full 80/20 T-slot table for work holding and to give the machine some added weight for stability.

My questions are in relation to seek and feed rates and depth passes.

First, I'm using Makercam and Gcodesender. I thought I knew the difference between seek, feed and plunge rate, but perhaps the software is being weird. It seems ideal to set several rates:

1) Speed for moving the machine quickly across the table, and moving the Z-axis upwards
2) Speed for X/Y movement when milling
3) Speed for plunging (moving the Z-axis into the part)

Can these be set separately? It seems like no matter what settings I use they all end up being the same speed.

My second question is about milling speeds. I'll mainly be milling die-cast aluminum, but also wood and plexiglass. I have solid carbide plexiglass router bits, and two and four flute solid carbide high-temp long-life coated end mills (working temp of either 750F or 1400F). Very nice ones. It seems like all the machining I've seen done (including this: http://blog.inventables.com/2013/11/mil ... oko-2.html) uses depth passes of something like 0.1mm with a 500mm/min feed rate. That means it would take about 16 passes to cut through 1/16 of aluminum. To me that seems ridiculous and that cutting would take forever. It seems that if I was cutting with the DW660 by hand I'd naturally go waaay faster than that. Like for wood you'd just plunge straight in and cut through a 1/4" piece in one pass. And if drilling a hole in aluminum with a simple plunge cut, at 30,000rpms I'd just go straight through in a couple seconds, not .1mm at a time.

Are these numbers just extra cautious? Or maybe someone could explain better the idea behind all this?

WillAdams
Posts: 8488
Joined: Mon Apr 09, 2012 6:11 pm
Location: Pennsylvania --- south of the Turnpike, East of US-15
Contact:

Re: Seek and Feed rates, depth passes

Post by WillAdams » Sat Nov 23, 2013 8:09 pm

The values in the wiki tend towards the cautious, and for stock machines w/ ~120 Watt rotary tool --- your machine should be able to go significantly faster --- look to posts / values by others w/ similar machines.

You should be able to test w/ a scrap piece, constantly increasing speed and depth of cut until milling suffers, then back off a bit for safety and use those values --- please share your findings here or on the wiki.
Shapeoko 3XL #0006 w/Makita RT0701 Router w/0.125″ and ¼″ Elaire precision collets
Nomad 883 Pro #596 (bamboo)

danimal
Posts: 332
Joined: Wed Mar 13, 2013 5:53 pm
Location: Colorado

Re: Seek and Feed rates, depth passes

Post by danimal » Sat Nov 23, 2013 11:17 pm

Your CAM software can set individual seek, feed and plunge rates independent of the gcodesender. This way you can adjust for different operations depending on your need throughout the job for each individual milling operation.

Sorry for the book that follows, but I just want to put my findings out there in hopes that it will answer some of the questions that I had when I started and will help others wade through the pile of information out there. The thing is that there is no one size fits all strategy for speed and feed rates. It depends on the job you are running and your individual needs for that piece. I have made a simplified method for myself that accounts for the variables that I found to be important from other feed calculators. All the feed calculators that I have found are for productions sized equipment and do not even have plastics or wood in the materials list.

What I found is that feed rates are a constant depending on the end mill, step-over and speed of rotation. Material does not matter. The reason it does not matter is because your machine power compared to the material characteristics has a very slim margin that really all boils down to chip-size and removal. If you have optimum chip size for your end mill your machine has plenty of power to twist the bit through plastics and other soft material. If you start throwing metals into the mix then it is a different story, and I am still researching this. Where you are most limited is the torque applied to your machine perpendicular to the z axis. This is why 90% of the modifications are dedicated to strengthen up the z axis. The stiffer machine the bigger load it can take and the bigger the bite of material it can remove. But your chip size is still limited to the mill type and size, so the only other adjustments that you can make are pass depth, and step-over.

Step-over: This also affects chip-size and therefore affects feed rates. Generally speaking your step-size controls your surface finish, especially regarding 3D milling operations because the ball end mill is used. This is by preference for the job that you are running, meaning that if you have some curvy 3D object that has tight tolerances and will be difficult to finish by hand afterword, then you want to have your step over minimized to produce the best finish possible. I think that I read somewhere that the limit of diminishing returns it roughly 15% of your tool with diameter, but I can not remember for sure. I usually run about 25 to 30% tool diameter per step-over with good results on most jobs. For a 1/8 end mill in a 660 I use .8 to 1.0 mm step overs for plastics

Pass Depth: Your pass depth is completely dependent on your machine. The stiffer it is and the more power full the spindle, the deeper pass you can accomplish accurately. The harder the material the shallower the pass will be to prevent overloading the machine; ultimately missing steps or causing deflection resulting in poor finish quality. Another thing to consider is material placement. The further away the spindle gets from the center of the gantry (x axis) the more torque it applies to the axis causing more deflection.

My method for running a job on my shapeoko:

1) Determine how nice the finish needs to be. You trade time for finish quality, and some parts just don't need to be that pretty. This tells me my step over.

2) Using step over from above I select the mill that will do the job best, and I plug that tool information into my CAM software which gives me a ball park feed speed. I am using HeeksCNC currently, but I am trying out a couple other software packages that do a better job at 3D. Mu speed usually is between 650 and 850 mm/min for plastics.

3) Using the speed given above I start with a shallow pass of about .5 mm on the material that I am using. I have a little square circle cut that made as a default job for this test. I measure the results and make sure the machine cut through without any issues or visible deflection.

4) I return to zero.

5) I run the same job with a 1.0mm pass. I look closely for any signs of deflection, mostly that there is not a difference between the first and second pass. There will be a little ridge visible at the corners and along any axis that was over stressed. If this is not present I might run a 1.5 mm pass, but in general 1.0 does a good job and most things that I cut are between 3- 10mm thick. 10 passes at the above speeds does not take that long.

6) Set a new zero and run the job.
Shapeoko # 1458

RT0701C Spindle || dual y motor || x axis nema23 with custom carriage 1000mm length || z axis nema23 linear rail upgrade with 1/2-10 ACME

danimal
Posts: 332
Joined: Wed Mar 13, 2013 5:53 pm
Location: Colorado

Re: Seek and Feed rates, depth passes

Post by danimal » Sun Nov 24, 2013 6:16 pm

Also one thing to note, the top speed of the machine is mostly limited by the acceleration value. After a certain point it no longer travels any faster because it reaches the end of travel prior to reaching full speed. But if you adjust the acceleration value in gcodesender there is a limit where the stepper motors starts to miss steps particularly on the z axis. This is bad because it generally misses more steps on upward motion due to the slower speeds of the rapid safety clearance and the plunge speed going down.

This means the machine will think that it is higher than it really is and will plunge deeper than it should possibly with terrible consequences. I was running a multi-part job and on the first on it was perfect. The second one I heard it bog down a little on the first pass but then everything seemed fine and on the third part it tried to do a 4mm deep initial pass and I had to e-stop the machine. The gcode was correct, I was just progressively missing steps at a greater and greater rate as work was done. I had set the acceleration and seek speeds just a little too high and as the job progressed it got worse, possibly because things started to heat up. Moral of the story is, if you are concerned with reaching your max seek speeds to minimize production time, you will need to develop some sort of standard job to run that will determine if you are missing steps anywhere.

I am making up one now that has 5 slots cut with five passes each and I am setting the clearance height to 20mm so that it really works the z axis. Then I can run it and measure each finished slot with a depth micrometer to determine if any steps were missed. I also increased the current through the z axis motor slightly to give it a little more torque. It will just take some tweaking, but once you have seek speeds set you should not have to mess with them.
Shapeoko # 1458

RT0701C Spindle || dual y motor || x axis nema23 with custom carriage 1000mm length || z axis nema23 linear rail upgrade with 1/2-10 ACME

monkey123
Posts: 35
Joined: Sun Sep 08, 2013 3:36 am

Re: Seek and Feed rates, depth passes

Post by monkey123 » Sun Nov 24, 2013 9:56 pm

Thanks for all the tips! Interesting point about the acceleration values.

Is there a way to just make the Z-axis go up and down slower, and the X/Y accelerate and move quicker? I bumped up the speeds and the X/Y were moving very nicely, but the speed of the Z scared me a bit. Haha! And that was without the spindle going. I'd hate to see it accidentally plunge into something way too far and fast with a sharp bit at 30k rpms.

cvoinescu
Posts: 4442
Joined: Thu Jul 19, 2012 6:50 pm
Location: Camberley, UK
Contact:

Re: Seek and Feed rates, depth passes

Post by cvoinescu » Sun Nov 24, 2013 11:14 pm

With GRBL 0.8, you can only have one acceleration value for all axes. You're also stuck with the same speed for all axes, but some CAM packages allow you to use feed moves (G1) for all Z moves, including traverse moves (normally G0), so that you can set your traverse speed for the Z axis in CAM instead of GRBL. If your CAM can't do that, it's relatively easy to do in a G-code post-processor, but that's an extra step in the workflow.

GRBL 0.9 fixes this limitation, but it's still experimental.
Proud owner of ShapeOko #709, eShapeOko #0, and of store.amberspyglass.co.uk

Llamas
Posts: 201
Joined: Fri Apr 19, 2013 3:36 pm

Re: Seek and Feed rates, depth passes

Post by Llamas » Mon Nov 25, 2013 4:04 am

I don't know about other controller software, but grbl controller had an option to limit the z-axis speed to 260.

Sent from my SAMSUNG-SGH-I317 using Xparent BlueTapatalk 2

cvoinescu
Posts: 4442
Joined: Thu Jul 19, 2012 6:50 pm
Location: Camberley, UK
Contact:

Re: Seek and Feed rates, depth passes

Post by cvoinescu » Mon Nov 25, 2013 11:46 am

Despite the name, GRBL Controller is not the controller I had in mind. The controller is the Arduino running GRBL. GRBL Controller is, technically, "host software", interfacing the PC to the actual controller (GRBL). Its main job is to send the G-code over to GRBL, but, apparently, it can do G-code processing too. To limit the Z speed, it replaces G0 Z moves with G1 with an F argument, which is exactly what I was talking about.
Proud owner of ShapeOko #709, eShapeOko #0, and of store.amberspyglass.co.uk

Post Reply