Okuma Lathe Internal Thread Output causes crash

[jachattin]

  There needs to be a change to the threading options to prevent crashes!! Even though you select the bore on an internal thread, when doing left-hand threading when it is done it will raise and go through the part even though the graphics show it going out where it should. When you select LH thread, it should add a line right after the canned cycle to add a G0 Z.2 to get the tool out of the bore. As is, it goes back to the start of the thread cycle and lifts, which is through the part.

[Andrew_Todd]

Hi. Would you be able to share your Fusion file here so I can take a look for you?

File > Export > Save to local folder, return to this thread and attach the .f3d/.f3z file in your reply.

[jachattin]

I have attached an example using the same settings I used before.  I chose LH thread. I use Okuma post-process. I did a search on Google and on a mastercam forum somebody had the same issue, their solution was to insert a G0 Z.2 after the thread cycle because it happened to them. I did this and ran the program with no part and it worked. Without the G0 Z.2 it would go to the beginning of the thread in the bore then rapid up in X.

I tried both ways of selecting use cycle and unselecting cycle.

[Andrew_Todd]

Hi. We had a compny holiday yesterday so Im only getting to look at this now. If you can give me a few hours I will take a look. It looks like a post processor issue. 

[Andrew_Todd]

Are you able to send the post you are using and also show me the part in the code where the machine is crashing? Thanks.

[jachattin]

I have attached a copy of the program output, I am using the Okuma Post. 

(THREAD1)

N120 M1

N121 T090909

N122 G90 G95 G18

N123 M8

N124 G97 S500 M3 M41

N125 G0 X0.6 Z0.1969

N126 G0 Z-1.

N127 G71 X0.879 Z0.1969 D0.126 H0.07 F0.05906 M32 M73

N128 X0.6 Z0.1969<<<<<< This will crash the output should be G0 Z.1969

When you select the left-hand thread, and the inside bore, it should automatically know to move to clearance and then to a Z out of the bore, which is my point. 

[Andrew_Todd]

Ok. So N127 is the line with the threading cycle. Once the threading cycle completes the tool is still inside the bore? At what position?

[jachattin]

I believe it is at Z-1.00 then it goes up in X, which is in the bore. It seems it does not read the line below it. It does read the G0 Z.2. After it broke my part off, I ran it without anything in it, and it went back to Z-1. then up in X. So I went back to Fusion, looked over my selections, looked at the machine simulation, and then searched on Google. I found on the mastercam forum that the same situation happened, and a forum user suggested adding a rapid to Z clearance right after the cycle. They said it worked, so I did that and ran it without a part, and it moved to z clearance out of the would be bore. So thereafter I was able to run the parts. 

[Andrew_Todd]

I have open an internal ticket to get this fixed. Thanks for alerting us and sorry about the crash!