[carla]

Hi everyone

I am an engineering student here in the UK and have been given a CNC part program assignment. I have never had anything to do with CNC's before, so was hoping someone might be able to help or point me in the right direction.


Please see attachment 1) CNC part drawing attachment 2) CNC part programme.


The outside profile does not need to be machine and the part will be held in a machine vice. Although one would not normally start with machining the holes, I decided to write the second part of the program, first, so I could become accustom to writing a CNC program.

For the centre hole and inner profile, I assume that I will need to use an end mill and the codes G02 and G03, but I just don’t know what methods should be used to machine the part and how to write this part of the program. For example, will I need to machine the hole using ramp in/ramp out circular interpolation and for the inner profile, where should I start and do I need to use I, J and K? etc, etc, etc.

(All dimensions are in mm)

Any help would be very much appreciated

carla :bat:

[HuFlungDung]

Wow, you need to take a course to understand all that needs to be done. Oops, you are taking the course

Do they let you run your code on a real machine, even cutting air? That is the best way to learn.

With regard to your hole drilling routines, I've never used polar coordinates but I can kind of see the logic to it, and suppose it would work.

Some of your feedrates are a bit extreme. The chipload is how far the cutting edge can progress for each revolution of the spindle. This would be in the order of .05 to .1 mm/rev, per tooth. A drill has two edges, so at 1160 rpm the feedrate should be .05 * 2 * 1160 = 116mm/min. Don't confuse the depth of cut with the depth of the hole. They are not related.

When tapping threads, the feedrate is calculated differently. The tap must be fed at such a rate that it advances at the same rate as its thread pitch. So a .05" pitch tap turning at 1326rpm, must be fed at a rate of .05 * 1326 = 66.3 inches/min which equals 1684mm/min.

G28 is not mirror image. It is "return to reference position".

So far as doing the center hole, I think drilling would be useful to open the hole. Drill undersize by a mm or two. Then, and get this, use tool radius compensation to interpolate the circle with an endmill in a second operation. This will get you an A+ on your report card

The actual profile of the hole can be programmed using G03 CounterClockwise arcs and G41 tool radius comp Left. Typically, plunge position the tool safely inside the arc (by the amount of its radius, plus a few thousandths radial clearance (because the hole is rough), make a linear movement from the plunge point to the profile calling the G41 on the same line, and then use G03 arcs round the hole. Be sure to move back to the start plunge point as you cancel tool radius compensation with a G40.

[Bear]

Welcome, to C.N.C.Zone ,
I cant help much,but,what kind of machine is this you are programing,
what kind of tooling do you have.With those speeds and feeds it must
be quite a productive machine.What kind of studies are you taking?
Bear (wedge)

[carla]

Hi there Guys.

Thank you for the help.

My course is a "BTEC Higher National Certificate in engineering Manufacture" and the subjects covered this year, are Mechanical principles (science), Computer Aided Engineering, Quality Assurance and Management, Materials, Project, and Business Management Techniques. This is a part-time course, that is, I attend college one day a week, but in reality, I spend most of the week studying. Also in reality, most of us students are self-taught, some of our lessons lack any real tutoring, which is a sad state of affairs really.

I will be required to input the part program, but do not believe I will be machining any material. Unfortunately I do not get the opportunity to practice on a real machine, infact I have not even seen it. I will ask the tutor what machine this is, and let you guys know.

Polar co-ordinates, I used this method as I am requires to create a part program to maximum efficiency and found this method slightly shortens the part program. As for the feedrates, yes, they are wrong and did think they where somewhat high at the time, but I am now in the process of correcting this, and a couple of other bits and pieces, such as the G28, Mirror image, which was stated in the G-codes given to me by my tutor, this sheet has now been filed, under rubbish, he, he.

As you stated in your advice, I have started to write the part-program for the large centre circle and the inner profile, so will see how I get on with this, although I still have a couple of questions:

How do I calculate feedrate for an M6, I assume this is a British method of describing a thread. I understand TPI, but don’t know how this works for an M6?

I also wanted to know, as the inner profile has short flats between each arc, I assume that I will need to use G02/G03 circular interpolation for the arcs then use liner interpolation for the straights and so on?

So again, many thanks for your help.

carla

PS: As part of the Computer Aided Engineering, I will be receiving an assignment soon, where I will be required to use the program called "Camtek, PEPS V5.3, Milling Module" so wondered if any one had a demo version of this software that I could use at home?

[HuFlungDung]

M6 has a pitch of 1mm, I believe, so this makes the feedrate calculation really easy. Just spindle rpm * 1mm = feedrate.

Yes, your inner profile will need to be programmed exactly for what it is. I could not see any flats, but you are correct in your plan. If it helps, the usage of G02 or G03 is subjective, because it is relative to the direction you plan to send the tool around the profile. The same thing applies to selecting G41/G42 tool radius compensation. The preferred technique is to have the cutter "climb milling". So when profiling inside a hole, the tool should orbit within the hole in a CCW (counter-clockwise) direction. On the outside of a profile, the tool would go round the profile in a CW direction.

[Navigator]

As by me programm should be changed. Don't need G20 for each tool,don't need G54 for each tool,if your clamps go above the part use G98... after each tool work put M00,or even better M01,it depends...

[cdlenterprises]

With a metric thread, the first number is the O.D. of the thread and the second number is the pitch of the thread in mm. For example, an M12 X 1.75 thread would have a major dia. (O.D.) of approx. 12 mm and pitch (distance between two threads) of 1.75 mm. The way to program this on an machine using inch units would be to convert the metric pitch(in this case the 1.75) to inches. A common method is to multiply the metric value by .03937. This would equal .06889 inches which could be used for the feedrate in the program. As far as the mirror image goes, most machines I have seen use G51. It's optional on some machine controls so it may vary by machine. Hope this helps.