Re: [CAD_CAM_EDM_DRO] Please take a look o ver my shoulder – CAD CAM CNC Bench Mill System

Les, thank you. You have solved the last 1/3 of my system problem. I will
be using SheetCam. Your discussion of 2D and 2.5D machining, relating to
engraving was very informative. I learned a lot. Conceptually, I think
that when I enable a 4th rotational axis, that it will be replacing the
linear y axis to enable ring engraving. Your discussion pertaining to, 4)
"Load the G-code into your machine controller", finally allows me to
understand, what I call the translator, how the G code drives the chopper
controller. Your comments on software and mechanicals (torque requirements)
are also very useful.

You may be interested in my response to Jack. Jack solved the first 2/3 of
my systems problem by introducing me to KDN Tool & Automation Co, of Warwick
RI. They provide a complete mechanical (including no backlash ball screws),
electronic, and stepper motor solution for the SIEG X1, X2, and X3 Mini
Mills. I have the SIEG X2, Micro Mark #82573.

Again thank you for taking the time to help me out.

Whelen

----- Original Message -----
From: "Les Newell" <lesnewell@...>
To: <CAD_CAM_EDM_DRO@yahoogroups.com>
Sent: Friday, July 01, 2005 7:26 AM
Subject: Re: [CAD_CAM_EDM_DRO] Please take a look over my shoulder – CAD CAM
CNC Bench Mill System


> Hi Whelen,
>
> Wow, you have managed to ask a lot of question in one posting :-) OK,
> I'll do my best to help.
>
> First CAD/CAM. Think about the sort of work you want to do. You
> automatically assumed you need 3D CAD/CAM. Do you? 3D is great for mould
> making and 3 dimensional carving but it is not ideal for more
> 'conventional' work such as engraving or general purpose milling. Quite
> a few people have bought expensive 3D packages and found out they are
> better off with 2.1/2D. Could a skilled machinist cut the parts you
> want, assuming he/she could operate both X and Y handles at the same
> time (Or X and A for a rotary axis)? If so, you only need 2.1/2D. With
> 2.1/2D machining the Z axis does not move with the X and Y. This is like
> most manual milling. You set the cut depth then take some cuts, change
> the depth then take some other cuts and so on.
>
> With engraving it is often a good idea to use a 'floating head'. The
> cutter holder is mounted on some form of slide mounted on the Z axis so
> it can freely move up and down with a light spring to push it down. The
> cutter projects through a guide nose that touches the work and controls
> the cut depth. Any variations in the surface are followed by the guide
> nose, keeping a consistent cut depth. You can engrave onto curved
> surfaces using this technique. In extreme cases there are guide noses
> available that use a ball with a hole drilled in it. The ball is free to
> rotate in any direction and the cutter runs through the drilled hole.
> This will follow even quite steep angles. You could instead use a fixed
> cutter and use 3D CAD to draw the part you are cutting but your drawing
> will have to be very accurate. For instance if you are engraving .005
> deep, your drawing will have to be accurate to 0.001", not easy
> especially if the ring is hand made and not perfectly accurate.
>
> For normal engraving you would probably be better off with a good 2D
> 'artistic' CAD package and 2.1/2D CAM. A lot of engravers use CorelDraw.
> It is relatively cheap and has a huge array of text handling facilities.
> Combine that with a good CAM package and you will be able to do pretty
> much any engraving job. Corel's big downfall is that it is not great for
> precision engineering work. For that you are probably better off with a
> more conventional CAD package. DesignCad Express
> (http://www.upperspace.com/) is ludicrously cheap at $35 and is actually
> quite good. One nice feature of DesignCad is that it comes with it's own
> single stroke fonts that engrave really well. Ordinary Windows TrueType
> fonts don't engrave well if you are doing small work.
>
> For CAM I would suggest giving SheetCam (www.sheetcam.com) a try. It is
> $150 and works very well with CorelDraw or most other 2D CAD packages. I
> admit I am slightly biased here, being the author of SheetCam.
>
> Your best bet is to download all the demos you can get hold of and have
> a play. Software that suits one person may not suit another. Try to find
> something that you find easy to use.
>
> If you have the choice between stl and dxf, I would choose dxf. DXF
> files fully describe the whole object. For instance if you draw a circle
> a DXF file will specify a circle. STL files just describe the surface as
> a mesh of triangles in 3 dimensional space. A circle will be
> approximated by a large number of triangles joined together. This makes
> things a whole lot simpler for the CAM software but does reduce accuracy.
>
> You don't appear to be too sure how all the software components mesh
> together so here is a basic workflow which may clear things up a bit.
>
> 1) Draw your part in CAD. This could be a 3D model or a simple 2D
> drawing. It helps to keep in mind how you are going to machine the part
> as you draw it!
>
> 2) Import the drawing into CAM and apply the tool paths. The CAM takes
> your drawing and works out where the cutter has to run to machine the
> part you have drawn. You have to provide a fair amount of input
> specifying how you want the part cut and what cutters to use. Your
> machining experience will help a lot here.
>
> 3) Once you have created the tool paths the CAM uses a built in program
> called a post processor to generate the G-code file. G-code is just a
> sequence of movement instructions for your machine. G-code gets it's
> name from the instructions, most of which start with the letter G. Some
> instructions use the letter M but they are still called g-code.
>
> 4) Load the G-code into your machine controller. This can be a dedicated
> machine or software running on your computer such as
> Mach2(www.artofcnc.ca) or Turbocnc (www.dakeng.com). The machine
> controller takes the g-code and converts it into electrical signals to
> the motor drives to actually move the machine. It also takes care of
> jogging, zeroing coordinates, coolant etc.
>
> On to the mechanical side:
>
> How much torque do you need? This is the most difficult question. It
> depends very much on your machine. Think of how much torque you have
> needed to apply to the handles when using this machine. Estimate the
> maximum you have ever needed to apply while taking a heavy cut. Use this
> as the continuous torque rating of your servo drive system. This is a
> very conservative estimate but you are better safe than sorry. Once you
> have this torque, find out what the continuous rating of your motor is.
> The ratio between these two values will give the reduction ration
> needed. For instance if you estimate you need 400oz-in to turn the
> handle and your motor is 100 oz-in then you need 4:1 reduction. Toothed
> belt is ideal because it gives you the option to easily change ratios if
> you get it wrong. Your rapid speed will be the motor maximum speed
> divided by the reduction ratio times the screw TPI. Say the motor can do
> 4000RPM and your screw is 10TPI. The rapid speed will be 4000/(4 * 10) =
> 100IPM - this would be plenty fast enough.
>
>
> Should you replace the lead screw nuts? Possibly if they are worn. You
> want to do everything possible to reduce backlash. Ideally you should
> replace the screws with ballscrews as CNC machines are less tolerant to
> backlash than manual machines. Theoretically the software can compensate
> but in practise it is not an ideal solution. Ballscrews are expensive so
> I would suggest running with the current screws for the time being. The
> machine will work with them so you can upgrade in the future if you find
> the backlash is a problem.
>
> Should you loosen the gibs? NO! Keep them just loose enough to move
> freely and use plenty of good quality slideway lubricant (not engine oil).
>
> Should you lap the ways? Would you if you were keeping the machine for
> manual use? Lapping should be done with care or you can make things
> worse rather than better.
>
> I hope that has helped answer some of your questions,
>
> Les
>
>
> Addresses:
> FAQ: http://www.ktmarketing.com/faq.html
> FILES: http://groups.yahoo.com/group/CAD_CAM_EDM_DRO/files/
> Post Messages: CAD_CAM_EDM_DRO@yahoogroups.com
>
> Subscribe: CAD_CAM_EDM_DRO-subscribe@yahoogroups.com
> Unsubscribe: CAD_CAM_EDM_DRO-unsubscribe@yahoogroups.com
> List owner: CAD_CAM_EDM_DRO-owner@yahoogroups.com, wanliker@...,
> timg@...
> Moderator: pentam@... indigo_red@... davemucha@...
> [Moderators]
> URL to this group: http://groups.yahoo.com/group/CAD_CAM_EDM_DRO
>
> OFF Topic POSTS: General Machining
> If you wish to post on unlimited OT subjects goto:
> aol://5863:126/rec.crafts.metalworking or go thru Google.com to reach it
> if you have trouble.
> http://www.metalworking.com/news_servers.html
>
> http://groups.yahoo.com/group/jobshophomeshop I consider this to be a
> sister site to the CCED group, as many of the same members are there, for
> OT subjects, that are not allowed on the CCED list.
>
> NOTICE: ALL POSTINGS TO THIS GROUP BECOME PUBLIC DOMAIN BY POSTING THEM.
> DON'T POST IF YOU CAN NOT ACCEPT THIS.....NO EXCEPTIONS........
> bill
> List Mom
> List Owner
>
>
> Yahoo! Groups Links
>
>
>
>
>
>
>