Questions on CNC Operations

Discuss tools and how to use them here.

Questions on CNC Operations

Postby dave49 » Mon Nov 26, 2012 2:00 pm

I work with Sherline mill and lathe, which I control manually. I am trying to envision how parts can be made under CNC control.
My mill has perhaps 0.006 inch backlash on the 3 axis leadscrew-nut sets. When controlling manually, it becomes reflexive to take out this backlash whenever positioning an axis, and then to set the travel locks on the axes that will not be used for the cut.

What happens on a CNC setup?
1. Is it unrealistic to expect to run under CNC a mill that has 0.006 backlash?
2. Must one consider only machines with preloaded ball leadscrews? Are such machines within the range of a hobbyist?
3. When writing g-code, it would be possible to plot moves such that backlash is taken out. But it seems to me much more difficult to plan for load direction changes that might lash. Does anyone have a solution for this?
4. Some CAD systems produce g-code that is "ready to use". Do these have any backlash compensation?

This whole business is quite a mystery to me. Any help would be appreciated.
Dave
User avatar
dave49
 
Posts: 75
Joined: Mon Apr 26, 2010 6:48 am
Location: Grayling MI

Re: Questions on CNC Operations

Postby eclecticguy » Mon Nov 26, 2012 4:53 pm

Hi Dave, I feel somewhat qualified to offer my input! I've built a CNC router from scratch, converted an X2 minimill and a Grizzly G0704 mill, a Sherline lathe, and a mini lathe. I'm contemplating converting my Grizzly G0602 10x22 lathe next. All except the router (I sold it before I got into reelsmithing) are used to make parts for my reels and reel kits. I've made parts for well over 1000 reels on these machines so I have developed some experience!

Firstly, while ball screws are nice (especially for rapid movements) you can use stock acme screws with no problem. My Sherline lathe is stock acme and my first X2 conversion used the stock acme screws. Backlash is an issue with all mechanical systems and 0.006" is not a show stopper (see below).

Answers:

1) not at all. Firstly, there are several software processes used to take an idea to a CNC'd part:

CAD -> CAM -> gcode -> Machine Controller

For this answer, I'll focus on the Machine Controller: there are really 2 options, Mach 3 (commercial but inexpensive) and EMC (open source). There are others but by far these are the most widely used and supported with large communities. Production machines use Mach 3 as well. The controller takes the gcode (the program that moves the cutter to shape the part) and controls the machine (mill, lathe, router, etc). These programs have automatic backlash compensation features that can be used to manage backlash. You do not do that in your CAM or gcode directly - those should be relatively machine independent. In addition, there are enhancements you can make to your machines to improve backlash - better couplers, double nuts, adjustable nuts, etc. I had the backlash on my X2 using stock screws and homemade Delrin adjustable nuts down to .002" on all 3 axis.

The other thing to note is "where do you need the precision?". 0.006" is really not that much. For frame perimeters and porting of frame and spool plates you don't need extremely high precision. For spool perimeters and the ID of frame openings, you can either live with it, cut them a bit oversize and finish on the lathe, or use a rotary table on the mill to cut them. A rotary table on the mill cutting disks or rings is not affected by backlash since the cutter is at a fixed location.

2) No, see my comments on my X2 with stock acme screws. However, ball nuts and screws are well within the reach of hobbyists. An X2 mini mill can be converted to CNC with kits (I used CNCFusion) and electronics packages for less than a CNC Sherline mill. The more work you can and are willing to do yourself, the more you save. I did all of the work on my original X2 conversion - machined the stepper mounts and other parts using the machine manually, put together my own electronics components , etc. When I decided to upgrade to ball screws, I choose the CNCFusion kit simply because I could not afford any down time from making parts. I did the conversion of my G0704 from scratch using plans from the guru on the CNCZone, Hoss.

3) you can write gcode manually but that is usually machine generated by your CAM program. Typically, you do not put backlash compensation moves into gcode. That is a function of the machine controller. Backlash is dynamic and you do not want to have to edit/re-write your gcode in 6 months when backlash on your machine changes. The automatic compensation in Mach is sophisticated and works well.

4) You won't find a CAM application that generates backlash compensation for the above reasons.

So, let me briefly describe the other software components:

CAD - this is where you design your parts. For my work, I can get by with what is called 2.5D, not full blown 3D. This is much simpler to draw and is a much less expensive software chain. Basically, it is like 2D drawing with "depth" (which is the Z axis on a mill). The CAD program needs to be able to output a standard format that the CAM application can read. The DXF format is most commonly used for 2 and 2.5D and can be used for 3D too. STL is also commonly used for 3D and somewhat for 2.5D. Almost all CAD apps I've used support these formats. Once you have drawn your part, you export it as DXF.

CAM - this takes the DXF file and provides the tools you need to create machining paths for your mill (or lathe). For instance, you set the tool properties (end mill, ball mill, etc, diameter, # flutes, IPM (inches per minute cutting speed), etc) and select a tool to actually make the cut. For instance, you might use a 1/8" end mill to cut the profile of a frame plate and a 1/16" end mill to cut the porting and drills to do the drilling operations. CAM allows you to set the speeds and feeds for the tool and materials that you are machining. There is a bit of an art to CAM since there is no "one right way" to do it. Once the tool paths have all been defined, you export them as what's called gcode. This is the universal machine instruction code used by most CNC mills and lathes.

Finally, you need a machine controller to actually move the machine. It's job is to translate the gcode (move from point x,y to x1,y1 at suchandsuch a speed) to the signals used by the electronic controller connected to the machine. The Machine Controller also does things like enable/disable coolant if you have it, backlash compensation, etc. Many controllers have "wizards" that generate the gcode for simple repetitive operations like milling a pocket or drilling a hole.

I've evolved my software as my production needs required but I started with a very cost effective commercial set of applications on the PC:

ViaCAD 2 & 3D
CamBam - CAM
Mach 3 - Machine Controller

The only change I've made is I now use VCarvePro instead of CamBAM. It has some simple drawing tools also so many things I can do directly in it without using CAD.

Hope this all helps!

Here's a video I made earlier this year porting reel parts on my X2 minimill under CNC control:



cheers,
Michael
My blog: www.EclecticGuy.com
The Reelsmith's Primer, reelsmithing materials, reels, lines and other items: www.EclecticAngler.com
User avatar
eclecticguy
Site Admin
 
Posts: 1161
Joined: Tue Jul 21, 2009 9:30 am
Location: New England, USA

Re: Questions on CNC Operations

Postby eclecticguy » Mon Nov 26, 2012 5:07 pm

Forgot to mention:

There are some very nice CNC routers available (and they are easy to build) that are great for 2.5D work and because they use a high speed router spindle, are super for milling aluminum with small bits. Many of us have small routers attached to the heads of our mills for doing detail work with small bits.

These machines have the added advantage that they have large X-Y platforms for milling more or larger parts.

The other thing to mention is the 3D printing technology has a lot of similarity to CNC machining. You can get a complete 3D printer setup for about $600 as a kit and start making parts. You can also put a small router on this machine to do machining. They have a work envelope of 6"x6"x6". I have two SeeMeCNC machines and they are great little devices. The software for these is all open source too.

cheers,
Michael
My blog: www.EclecticGuy.com
The Reelsmith's Primer, reelsmithing materials, reels, lines and other items: www.EclecticAngler.com
User avatar
eclecticguy
Site Admin
 
Posts: 1161
Joined: Tue Jul 21, 2009 9:30 am
Location: New England, USA

Re: Questions on CNC Operations

Postby eclecticguy » Mon Nov 26, 2012 5:17 pm

And another thing!

My response above was biased on milling. On a CNC lathe, most cutting operations are towards the spindle and either "in" or "out". Backlash is much less of a problem in these cases. Only complex lathed geometries would be affected and then backlash compensation can help.

cheers,
Michael
My blog: www.EclecticGuy.com
The Reelsmith's Primer, reelsmithing materials, reels, lines and other items: www.EclecticAngler.com
User avatar
eclecticguy
Site Admin
 
Posts: 1161
Joined: Tue Jul 21, 2009 9:30 am
Location: New England, USA

Re: Questions on CNC Operations

Postby dave49 » Mon Nov 26, 2012 9:37 pm

Michael,
Thank you for taking the time to provide so much information.

I did not know about the CAM layer of software; now many things are explained. This is the place in the design sequence where things like tool advance per pass would be set.

You did say a something that I did not understand: "automatic backlash compensation". I can see that if your stepper motor driven mill also had position transducers working directly on the slides, then a controller routine could measure the backlash. But I thought that the typical CNC mill did not include such transducers. How does the machine controller "automatically" compensate for backlash? (If I told it what I thought the backlash was, it might do open loop compensation.)
Regards,
Dave
User avatar
dave49
 
Posts: 75
Joined: Mon Apr 26, 2010 6:48 am
Location: Grayling MI

Re: Questions on CNC Operations

Postby eclecticguy » Mon Nov 26, 2012 9:45 pm

Dave, it is actually open loop but the vendors call it automatic backlash compensation. You measure the backlash on each of the axes and tell the software these measurements. The software (at least Mach) uses a notrivial algorithm to apply the compensation depending on how fast the tool is moving and it's direction on all 3 axes simultaneously (or whichever axes are involved in the movement).

Cheers,
Michael
My blog: www.EclecticGuy.com
The Reelsmith's Primer, reelsmithing materials, reels, lines and other items: www.EclecticAngler.com
User avatar
eclecticguy
Site Admin
 
Posts: 1161
Joined: Tue Jul 21, 2009 9:30 am
Location: New England, USA


Return to Tools & Techniques



Who is online

Users browsing this forum: No registered users and 1 guest

cron