N# = T# For lathe.

[lamlinh]

Hi All,

 

I use MX5 with lathe post- mplfan. I want to have n# = t# for each tool in my lathe program. can someone helps me with my post?

 

Thanks.

[Chris McIntosh]

Your best bet would be to download the mplmaster for X5 from here: Mplmaster for X5

 

In the post there is a switch called tseqno, set this value to 2 in order to have the sequence numbers match the tool numbers and you're done!

 

In mplfan you would need to turn off sequence number output in the control def, then in the ltlchg$ and mtlchg$ post blocks set sequence number equal to the tool number (n$ = t$). After setting the sequence number force it out by putting a star in front of it where you would like the sequence number to be output(*n$).

 

HTH

[lamlinh]

Hello Chris,

 

Thank for the post and it works now. There is a problem with drill canned cycle. I set clearance .25 above the part and retract .1 obove the part, the post come out as following.

G83 Z-1. R-.15 Q2500 F.01 (R-.14 should be .1)

G80

and also my longhand drill is the same as above.

G83 Z-1. R-.15 Q2500 F.01

G80

For the longhand drill, subsequent peck, peck clearance and retract amount in the operation are grey out.

can you help me to modify the post.

 

Thank.

[K2csq7]

Did you select your retract of .1 above the part as absolute or incremental?

[Chris McIntosh]

By default the post has been setup to output the R value as an incremental distance from the clearance plane. In your case you are programming 0.25" as clearance and 0.1" as retract, so your output is 0.1-0.25=-0.15". It sounds like your control takes the R value as an absolute. If you are using the mplmaster post, there will a post block called prdrlout where you will need to uncomment a couple lines. Your post block should look like the block below with changes made to the final three lines:

 

prdrlout        #R drill position
     if mdrl_dir = zero,
       [
       refht_a = refht_z
       refht_i = refht_a - initht_z
       ]
     else,
       [
       refht_a = refht_x
       refht_i = (refht_a - initht_x) / dia_mult
       ]
     if absinc$ = zero, refht_a, !refht_i  <--remove # from the start of this line
     else, refht_i, !refht_a               <--remove # from the start of this line
     #refht_i, !refht_a            #Fanuc is always incremental from initial height <--add # to the start of this line

 

The long hand drill should be output as long hand drilling, not as a canned cycle as you have indicated. If you go into mastercam in the settings menu -> control def manager, under the machine cycles menu, select lathe drill cycles and ensure that the peck drill check box has been unchecked. This will output the peck cycle as a long hand cycle.

 

While still in the control def, going to the text menu and selecting lathe drill cycles, remove the double quotes from the subsequent peck and peck clearance cells to enable those fields.

 

Please let me know if you have any further issues. I'm going to look at the master on the server and see if the longhand has not been setup correctly.

[lamlinh]

Hi All,

 

Keith A-1. I selected retract of .1 above the part as absolute.

Chris.Thank alot!!!. Everything goes smoothly now.