584,798 active members*
4,434 visitors online*
Register for free
Login
IndustryArena Forum > WoodWorking Machines > DIY CNC Router Table Machines > Five tips for creating faster and more efficient tool paths for your CNC wood router
Results 1 to 13 of 13
  1. #1
    Join Date
    Aug 2011
    Posts
    0

    Five tips for creating faster and more efficient tool paths for your CNC wood router

    Hey everybody. I finished my DIY router table about 9 months ago, and looking back I would have appreciated the following tips as I was getting familiar with CAM programming for a wood router. It might be rudimentary stuff to some of you, but hopefully it's helpful to some beginners.

    The version with screenshots can be read here.

    Five easy tips for creating faster and more efficient tool paths for your CNC wood router

    by Matt Dylan Street

    Firstly, let's define the term efficient when talking about a CNC tool path. An important part of the CNC milling process is the tricky balancing act of getting the job done faster vs. making your tools last longer. If you don't mind buying new end mills after every other job, then by all means, run your machine as fast as it'll go; but if you loathe spending big bucks on tiny pieces of tungsten carbide, then take it easy and just cruise along at 3 IPM. As I'm sure you know, both of these scenarios are completely impractical. This dichotomy illustrates just one of the many plights of the CNC machinist. The following five nuggets are what help me achieve what I consider to be a good balance in my own shop, and I hope you and your shop can benefit from reading.

    Please note that this guide is geared toward FeatureCAM software, which is what I use most of the time, so the terminology might not be familiar to you if you use a different CAM package such as MasterCAM or BobCAD-CAM. However, these tips are universal CAM principles and can be applied to most other CAM programs.

    So, without further ado, let's get on with the list:

    #1 Enable the minimize tool retract option.

    Minimize tool retract is a milling attribute in FeatureCAM that reduces the amount of retracting that the tool will perform while milling. Instead of retracting, the tool will continue feeding to its next location.

    Retracting and plunging more than necessary can add substantial time to your tool path. While retracting takes some time, the plunging is what really eats up time since the plunge feed rate is usually slower than the regular feed rate.

    This option is located in Manufacturing > Machining Attributes under the Milling tab.

    #2 Plunge, don't ramp.

    When leading in/out, select plunge to depth rather than ramp to depth or helical. This will again prevent a lot of unnecessary motion. Since we're milling wood with a center cutting end mill, easing into the stock with a ramping or helical approach is not necessary. The end mill will have no problem directly plunging into wood.

    If the operation supports it, this attribute can be found in the leads tab. For an operation such as side that does not have this tab, you can set the max. ramp angle to 0 in the milling tab.

    #3 Don't use the default Z increment.

    Z increment is the attribute in FeatureCAM for setting the depth of cut. This value is the maximum Z increment that will be used to rough the feature.

    If you're using a tool path that cuts to a certain depth, like a groove, side, or z level roughing, the default Z level increment that FeatureCAM selects for you will create more passes than you really need for wood milling. It makes sense that if you're milling a .5" deep groove in a block of aluminum, you would not do it in one pass at .5" deep. This would be too much for the tool to handle. Instead, you would want to use several passes at shallower depths.This is what FeatureCAM assumes when it calculates the default Z increment.

    Wood, however, is obviously much softer than aluminum; therefore, your carbide end mill can handle a much deeper pass without burning or breaking. Of course, this doesn't mean you can cut a 1" deep groove through a slab of oak at 120 IPM and not expect to fill your shop with smoke, and possibly start a fire. You'll have to get a feel for the depth you need based on the tool, feed rate, speed rate, and wood species you're milling. As an example, when I make a cutting board for Fat Bison Workshop, I cut all the way through the 1" maple stock with a side feature. I do this with an 1/8" end mill in two .6" deep passes at about 30 IPM.

    If the operation supports it, this attribute can be found in the milling tab.

    #4 Increase your stepover.

    Stepover is the distance between tool path center lines.

    When using a flat end mill, you can slightly increase your stepover % and still achieve the same result. FeatureCAM's default stepover value is 30% (this means the stepover distance is 30% of the tool's diameter). You should only do this with flat end mills since the tool's full diameter is cutting at the end. I sometimes increase this value to 50% with my .25" end mills, but I usually only bump it up to 35% or so for my smaller end mills.

    Even the smallest increments will help speed things up. Imagine you're cutting a rectangular pocket in horizontal passes with whatever end mill you want. If you just bump up the stepover from 30% to 36%, that 6% will save you one extra horizontal pass for every 16 passes. Considering some jobs have thousands of passes, the amount of time saved can add up to be quite respectable.

    If the operation supports it, this attribute can be found in the milling tab.

    #5 Max out your rapid speed.

    If your machine will travel reliably at 600 IPM, then by all means set that as your rapid traverse speed. There's no sense in leaving your machine’s capabilities untapped. This setting is usually made in your CNC software (i.e. Mach3) and not in the CAM software.

    #6 Bonus tip (FeatureCAM only)!

    Set the tolerance and finish allowance to 0 and FeatureCAM will calculate your tool path much faster. This is a FeatureCAM specific thing, and I'm not sure what it is about the program's tool path algorithm that causes this, but it works. It's most noticable when calculating a surface milling feature such as a .stl file. Note: If you're seeing strange behavior on flat surfaces when z-level roughing after setting these values to zero, try to resave your .stl in your CAD program with a lower tolerance (more precise).

    As I’m sure you know, the CNC machining process, from concept to-CAD to CAM to finished product, can be complicated to say the least. I hope these tips help you slightly uncomplicate the processes in your own shop.

    Thanks for reading, and please check out my shop and creations at Fat Bison Workshop and Fat Bison Workshop Custom Carved Wood Ranch Signs | Official Home.
    See some stuff I've made at fatbison.com and customranchsigns.com

  2. #2
    Join Date
    Aug 2011
    Posts
    0

    Thanks 5 Tips for reducing machining time

    There are all great tips, I have been able to implement on Meshcam and reduced my GCode line count from 64,000 to 19,000 for the same part with a very minor loss in finish.

    Stepover is a real big factor, as I was cutting pine wood, I went to max step over.

    Cheers

    John

  3. #3
    Join Date
    Apr 2009
    Posts
    5516
    Good thread! I'd like to add a few:

    Use the largest tool possible that will get the job done

    Aside from machines with smaller spindles, where the tool diameter is limited, you really can increase the speed of a job simply by selecting the largest tool that will work. You'll generally end up with a better finish since the larger tool is more ridgid; and consequently you can be more aggressive with it

    Set your contoller to CV (Constant Velocity)

    There may be a tine when you need this turned off. I haven't had to yet.

    Obtain chipload charts from your tool manufacturer

    You really can optimize the speed of your job and life of your tools by using the chipload charts as a starting point. The charts are based on a cut depth the same as the diameter of the tool. For a DOC 2X the bit diameter, you should decrease the chipload to 50%, and for 3X, 35%. The tool is more efficient at the flank as opposed to the bottom, so the deeper you can cut, the better. Also the closer the work is to the collet, the more ridgid the setup is.

    Spiral contour ramp-in if possible

    Amazingly, this is a feature in VCarve Pro. The tool will ramp in at the DOC stepover you specify, so you can do this move at full speed. You might even get a better wall finish in critical parts since the tool does not pause and plunge down. On holes less than 2X the diameter of the tool, I just spiral down (helix) instead of pocketing it.

    Multiple pocketing strategies

    It is usally faster to complete a pocket to depth before moving to the next one. Some CAM may run all pockets to one Z level, then start again, causing a lot of repetitive moves. If your CAM supports this, you can set it to complete each pocket before moving to the next. If there are not a lot you may do this manually.

    Use the right tool for the job

    While you can use some endmills on wood, they are not as aggressive as wood bits. Endmills have a totally different geonetry - less edge rake, smaller flutes - than wood bits. Ball endmills are usually fine since the cuts made with them are generally very small. As mentioned above, ball endmills are very inefficient for roughing since the tip has a zero diameter. If your using a bull endmill (radiused tip) you should adjust your stepover a percentage of the FLAT PART of the tip.

    Use bits with less flutes for high-rpm spindles

    I find that single-edge bits like single-edge compression spirals and O-flutes work very well with high-rpm routers on the CNC. They take larger chips which help draw heat from the tool and throw the chips away from the cut. Usually with multi-flute bits, even some 2-flute bits, you don't really gain any benefit until you cut at speeds more in the realm of commercial machines and way past the speed and ridgidity of most DIY machines. The spiral-"O"-flutes are also my weapon of choice for non-ferrous metals.

    As to #1 above, MAKE SURE your bit or endmill is center-cutting before plunging wiith it. There are many bits that are NOT, and these include many bits purchased at the big-box stores. Many mortising bits are NOT center-cutting, since the clearance in the middle is there by design to clear chips.

  4. #4
    Join Date
    Aug 2011
    Posts
    0
    Awesome additions louieatienza! I don't have my Mach3 in CV mode. I've never tried it. I just read that it could round out square paths. Do you notice this at all?
    See some stuff I've made at fatbison.com and customranchsigns.com

  5. #5
    Join Date
    Mar 2003
    Posts
    35538
    An important part of the CNC milling process is the tricky balancing act of getting the job done faster vs. making your tools last longer. If you don't mind buying new end mills after every other job, then by all means, run your machine as fast as it'll go.........
    Generally, the faster you go, the longer your tools will last. Cutting faster can result in higher chiploads, which results in cooler running bits, which will last much longer.
    When cutting non abrasive woods, the #1 cause of tools getting dull is heat, usually caused by chiploads being to low, either from too high rpm or too low feedrates.
    If you want your tools to last, faster is usually better.



    #2 Plunge, don't ramp.

    When leading in/out, select plunge to depth rather than ramp to depth or helical. This will again prevent a lot of unnecessary motion. Since we're milling wood with a center cutting end mill, easing into the stock with a ramping or helical approach is not necessary.............
    Even when cutting wood, plunging is not a good idea. One, it puts high axial loads on spindle bearings, which aren't designed for plunging. And two, it will generate tremendous heat at the tip of the tool, causing burning and shortening tool life.
    Gerry

    UCCNC 2017 Screenset
    http://www.thecncwoodworker.com/2017.html

    Mach3 2010 Screenset
    http://www.thecncwoodworker.com/2010.html

    JointCAM - CNC Dovetails & Box Joints
    http://www.g-forcecnc.com/jointcam.html

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

  6. #6
    Join Date
    Aug 2011
    Posts
    0
    ger21,

    Firstly, thank you for the valid points! If I'm saying some bunk stuff, I need to know.

    But please allow me to justify my statements for the sake of my pride.

    1. About running the machine too fast: I've nearly started a fire by feeding too fast. Faster is better for heat transfer via chip load to some extent, but nobody would argue there is such a thing as too fast. You can easily cross the line and run the tool faster than it can keep up with. I meant "as fast as you want" as in "as fast as you can."

    2. Speaking for myself, every tool path I make has minimal plunges. One plunge for a minute plus of pocketing, and then another plunge for the next pocket and so on. The time spent plunging, in my experience, is hardly enough to generate any notable heat. Again this is in my personal experience; I'm not plunging very deep or very often. It's not a fast plunge either. 50% of feed rate, but still faster than ramping. As far as the spindle not handling axial loads well, that depends on the type and brand of tool you're using. I've busted two router bearings in my short career, neither of which were busted during a plunge. Just think about your ratio of plunge movement vs. feed movement; my ratio might be somewhere around 1%, and that, in my opinion, is not enough to worry about axial load.

    I see you've had a ton more posts and therefore a ton more experience than me, ger21, but I just couldn't resist defending my thoughts. I'd love to hear some more opinions. I hate buying new tools!
    See some stuff I've made at fatbison.com and customranchsigns.com

  7. #7
    Join Date
    Apr 2009
    Posts
    5516
    Quote Originally Posted by steet81 View Post
    Awesome additions louieatienza! I don't have my Mach3 in CV mode. I've never tried it. I just read that it could round out square paths. Do you notice this at all?
    Not really, though I do have my accel set as high as I can...

  8. #8
    Join Date
    Mar 2003
    Posts
    35538
    1. About running the machine too fast: I've nearly started a fire by feeding too fast.
    I believe you're mistaken. Feeding faster will reduce the possibility of burning. Not increase it.

    If your feeding at a rate that is causing burning, slowing down will make it worse, and increasing the feedrate will decrease the burning. The exception may be with an extremely dull tool, but I don't think so.

    At what feedrate did you almost start a fire?
    Gerry

    UCCNC 2017 Screenset
    http://www.thecncwoodworker.com/2017.html

    Mach3 2010 Screenset
    http://www.thecncwoodworker.com/2010.html

    JointCAM - CNC Dovetails & Box Joints
    http://www.g-forcecnc.com/jointcam.html

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

  9. #9
    Join Date
    Apr 2009
    Posts
    5516
    Quote Originally Posted by steet81 View Post
    ger21,

    Firstly, thank you for the valid points! If I'm saying some bunk stuff, I need to know.

    But please allow me to justify my statements for the sake of my pride.

    1. About running the machine too fast: I've nearly started a fire by feeding too fast. Faster is better for heat transfer via chip load to some extent, but nobody would argue there is such a thing as too fast. You can easily cross the line and run the tool faster than it can keep up with. I meant "as fast as you want" as in "as fast as you can."

    2. Speaking for myself, every tool path I make has minimal plunges. One plunge for a minute plus of pocketing, and then another plunge for the next pocket and so on. The time spent plunging, in my experience, is hardly enough to generate any notable heat. Again this is in my personal experience; I'm not plunging very deep or very often. It's not a fast plunge either. 50% of feed rate, but still faster than ramping. As far as the spindle not handling axial loads well, that depends on the type and brand of tool you're using. I've busted two router bearings in my short career, neither of which were busted during a plunge. Just think about your ratio of plunge movement vs. feed movement; my ratio might be somewhere around 1%, and that, in my opinion, is not enough to worry about axial load.

    I see you've had a ton more posts and therefore a ton more experience than me, ger21, but I just couldn't resist defending my thoughts. I'd love to hear some more opinions. I hate buying new tools!
    1: The trick is to have the right spindle speed for your feedrate that will generate the proper chipload for the tool. Since the toolmaker will normally recommend the chipload, your spindle speed will determine the feedrate, so feedrate = chipload X spindle speed X number of flutes. So the faster you set the router speed, the faster you have to cut. If you must keep the spindle speed high you cna decrease the number of flutes. As for too fast, Onsrud does a demonstation where they cut 3/4" plywood in a single pass at 2800IPM, with a 4-flute high velocity compression spiral. I don't know of any DIY machine capable of rapids that high, let alone feedrates. No fires were started either!

    The big issue is that most DIY machines do not have the ridgidity or spindle power to meet even some of the minimum chipload requirements, and we compromise by taking either shallower cuts, higher spindle speed, lower feedrate, or a combination of the three. This is normally OK since most of us do not run out machines 8 hour shifts 365 days of the year. We also don't have 40HP spindles and 2HP servos on a cast iron frame. But the chiploads are at least a starting point to not only getting better tool life, but better cuts as well.

    2: If you think about it, you can ramp or helix in at full speed as opposed to plunging at half, and your material removal rate will be higher. You also don't bury the tool which can cause heat. Also, the tip of the bit is the most inefficient part of the bit, ramping will let you cut with more of the flank.

  10. #10
    Join Date
    Aug 2011
    Posts
    0
    Quote Originally Posted by ger21 View Post
    I believe you're mistaken. Feeding faster will reduce the possibility of burning. Not increase it.

    If your feeding at a rate that is causing burning, slowing down will make it worse, and increasing the feedrate will decrease the burning. The exception may be with an extremely dull tool, but I don't think so.

    At what feedrate did you almost start a fire?
    When I was starting out I probably ran it at about 160 IPM at a .5" depth. Could very well have been a dull tool also. My DIY machine uses a router that I can't change the speed on.
    See some stuff I've made at fatbison.com and customranchsigns.com

  11. #11
    Join Date
    Aug 2011
    Posts
    0
    louieatienza, That makes sense about the ramping when you put it that way.
    See some stuff I've made at fatbison.com and customranchsigns.com

  12. #12
    Join Date
    Apr 2009
    Posts
    5516
    Quote Originally Posted by steet81 View Post
    When I was starting out I ran it too fast. Probably 160 IPM at a .5" depth. Could very well have been a dull tool also. My DIY machine uses a router that I can't change the speed on.
    Methinks it's not fast enough! I don't think running too fast at too shallow a depth is good either, since you're just wearing out the bottom of the bit. But let's say you were using a 1/2" 2-flute bit, with a recommeded chipload of .005" and your router runs at 24kRPM. That would theoretically be 240IPM at 1/2" depth! But since the router would probably bog down under this load, and your machine may not be as ridgid or powerful as a commercial one, usually the first thing to do is keep the speed but decrease the depth until the machine can cut comfortably. If you have to cut too shallow at that speed then you decrease the feedrate.

  13. #13
    Join Date
    Aug 2011
    Posts
    0
    Thanks guys. I'm learning that my concept of feeds and speeds might need a little adjusting for my setup. You're right about the rigidity; my DIY gantry is not stable at higher feeds. You're right about the router as well; Us DIY guys are running relatively low HP routers that can't always hang.

    Update: I've changed the original blog post on my site to include the argument against plunging. I also removed my line about running it as fast as you want. Don't want to spread misinformation.
    See some stuff I've made at fatbison.com and customranchsigns.com

Similar Threads

  1. Creating Tool paths with a solid
    By Rathi in forum Mastercam
    Replies: 6
    Last Post: 07-22-2010, 04:04 PM
  2. creating cut paths for single line text
    By fitzy in forum Torchmate
    Replies: 6
    Last Post: 09-26-2008, 04:13 PM
  3. Creating tool paths
    By CNCMike in forum Mastercam
    Replies: 4
    Last Post: 04-15-2008, 09:38 PM
  4. efficient tool path
    By balsaman in forum Mastercam
    Replies: 32
    Last Post: 07-28-2006, 05:37 PM

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •