Topics

Help with code for compact 5 cnc

mastuart1@...
 

Hi I have been trying to use MFI to get the program for some parts that I what to make for a model engine I want to build.   The parts I want to make are the cylinders.  I have 24 blanks roughed out.  They are 1.625 dia x 2.156 long.   I have them faced on both ends and are the right length and they are bored.  I did this on a manual lathe. 

 

I now want to use my Emco compact 5 Mk4  to do more work on them.  I have been getting frustrated trying to punch in my program on the machine.  No matter what I do I keep getting alarm 02 when I type in my x number.  

 

It would be real helpful if someone  could write the code that I need .  I could then punch it into my machine and see if it works .  I could also put it into MFI  and see how it compares to what I have done.   This would be a big help to me understanding what I am doing.

 

 

I have  the machine set on inch mode.    I would like to use feed per rev for feed . I would also like to do this in absolute mode. I would like to use g84 to turn the 1.375 dia and the 1.250 dia.   After the turning cycle was done use g78 for the threading cycle.     Almost forgot the material is 12 L14  steel . It is leaded steel and cut like butter.   So use whatever feeds and speeds are appropriate.

   I will try to attach  a crude drawing .     Thanks for your help              

 Mark

 

 

mastuart1@...
 

I forgot to add my machine has the turret tool changer

 

Mark



---In Emco_cnc_users@..., <mastuart1@...> wrote:

Hi I have been trying to use MFI to get the program for some parts that I what to make for a model engine I want to build.   The parts I want to make are the cylinders.  I have 24 blanks roughed out.  They are 1.625 dia x 2.156 long.   I have them faced on both ends and are the right length and they are bored.  I did this on a manual lathe. 

 

I now want to use my Emco compact 5 Mk4  to do more work on them.  I have been getting frustrated trying to punch in my program on the machine.  No matter what I do I keep getting alarm 02 when I type in my x number.  

 

It would be real helpful if someone  could write the code that I need .  I could then punch it into my machine and see if it works .  I could also put it into MFI  and see how it compares to what I have done.   This would be a big help to me understanding what I am doing.

 

 

I have  the machine set on inch mode.    I would like to use feed per rev for feed . I would also like to do this in absolute mode. I would like to use g84 to turn the 1.375 dia and the 1.250 dia.   After the turning cycle was done use g78 for the threading cycle.     Almost forgot the material is 12 L14  steel . It is leaded steel and cut like butter.   So use whatever feeds and speeds are appropriate.

   I will try to attach  a crude drawing .     Thanks for your help              

 Mark

 

 

m.wg@...
 

Hi Mark


Just uploaded an MFI program to the Files section called Cylinder turn thread, ran OK on my machine but enter your tool offsets and number of tool jumps for the change.

Like you I had Alarm 02 with the X 1625 entered, just changed to 1624 throughout program and all was OK.

Max speed I found for the thread is about 480rpm.

Not sure what depth you need for the 24TPI thread but adjust as required.

If you go more than .030" you need to adjust the chamfer cut depth.


Working in mm units gives you better resolution and greater accuracy on size, MFI will convert program from inch to metric, or back if you want.

Hope this helps, Rgds, Marcus

mastuart1@...
 

Thanks Marcus for your help.    I got the program to work and just juggle the numbers some and got a part made to correct size.   I think I understand now what the problem was. It looks like some of the number of the diameter the program cant divide in half when it changes it to radius.     My machine has not been used in a

while and has developed a problem with the turret rotation.    I think I am going to take the motor off temporarily

and make a shaft and hand wheel to operate the tool changer until I can fix the control board. 

 I have another question or two .    Can I take my tool changer off and will a tool post like you have bolt on?

Do you know what kind of tools others are using to do internal threading and boring with the tool changer? 

Are they using round boring bars and threading tool mounted in the round holes in the turret?   If so where are they getting the tools that are the right diameter so you don't have to use adaptor bushings.   

One more question.  Are you using yours to do any cylinder finning?   I need to do 24 cylinders with 15 slots .031 wide .125 deep.    If so do you have any suggestion of  rpm for 1.375 dia leaded steel and what feed per rev.     

 

Thanks again Mark

m.wg@...
 

Hi Mark
I converted the program to mm and it functioned OK.

If you check in the Photos there are some pics showing the Emco standard tool post on a C5 lathe. There are 2 types, 1 has a central dovetail to secure in the block and the other an offset dovetail, both blocks are the same size but obviously the tool holders are not interchangeable.
Size of the block is 55mm square and 40mm high, there are 2 ground Vee's to accurately locate the toolholder so tool offsets remain constant between changes.
The block is mounted by a single M12 skt cap bolt to a 10mm thick plate which measures 60x80mm that is secured to the crosslide using the same fixings as the Auto tool turret with 4 M5x16 setscrews. 
For external threading I use a 12mm square Toolholder with replaceable tips but also have used carbide tipped tools on various size shanks.
For internal threads I use a selection of ground round section HSS for the smaller sizes, carbide tipped for larger and deeper bores., always try for the best rigid set-up and take very small cuts per pass, always use "springing cut" passes on internal threads as you do when boring.
The above statement is true for the Tool turret also, you can split any bushes you use to accommodate round tools in the turret socket, make sure the split is at 90 degrees to the tool securing screws before tightening then the split bush will clamp the tool securely. You may have to reduce the wall thickness on thick walled bushes by partly cutting lengthwise through the wall opposite the slit to allow closure.
Looks like you will have fun doing those fin cuts, .031" is going to be a delicate tool. All I can suggest is you grind the tools from square HSS stock leaving as much material below the tip as possible, grind the minimum length at .031" and only use a touch of clearance angles, top rake (7-10 deg ?) will help to form a nicely coiled swarf especially if kept lubricated. Set the tool at exact centre but if that doesn't work you may find better results with the tool a few thou below centre. Take some trial runs with the same material before putting your cylinders to the test, for starters infeed at 10mm/min using 200 rpm. Suggest you use G95 in case the tool jams, gives you the chance to manually back off.
Keep us informed reference feed rate and spindle speeds you finally use for cutting the fins.

Regards, Marcus