Bobcad post help

I'm trying to modify my post for a anilam 4200t cnc and when i post a program to do threads it gives me this

*TOOL #4 THREADING TOOL
T4
M41
G97 S600
G0 X1.17 Z.0575 M3
M8
G83 E0.0312 Z0.62 C0.01 D0.027 A60 S2
G0 X2. Z-.5625
G0 Z.1
M5
M2

I need the E to give me threads per inch instead of the decimal it is giving me.
If anyone could look at my post and tell me what i need to change to fix it I'd be greatful.

here is my post

2002. Program Block 2. Thread

PI = 3.141592653589793

ZLENGTH = LATHE_GetProfileStartZ() - LATHE_GetProfileEndZ()
XTAPER = LATHE_GetProfileStartX() - LATHE_GetProfileEndX()
LEAD = round(LATHE_GetThreadLead(), 4)
FIRSTPASS = LATHE_GetThreadFirstCut()
TDEPTH = cos((LATHE_GetAngleIn() / 2) * PI / 180) * LEAD
TANGLE = LATHE_GetAngleIn()
SKIMS = LATHE_GetFinishNumberOfCuts()
ZRETRACT = LATHE_GetRoughRetractAmount()
STARTS = 1

OUTSTRING = "'G83',"
OUTSTRING = OUTSTRING&"'E"&LEAD&"'"
OUTSTRING = OUTSTRING&"'Z"&Round(ZLENGTH, 4)&"'"
OUTSTRING = OUTSTRING&"'C"&Round(FIRSTPASS, 4)&"'"
OUTSTRING = OUTSTRING&"'D"&Round(TDEPTH, 4)&"'"
OUTSTRING = OUTSTRING&"'A"&Round(TANGLE, 4)&"'"
If SKIMS > 1 Then
OUTSTRING = OUTSTRING&"'S"&SKIMS&"'"
End If
OUTSTRING = OUTSTRING&"'R"&Round(ZRETRACT, 4)&"'"
OUTSTRING = OUTSTRING&"'X"&Round(XTAPER, 4)&"'"
OUTSTRING = OUTSTRING&"'W"&STARTS&"'"

CALL LATHE_ProcessPostLine(OUTSTRING)

Does not see the E section in your post.
Are you sure this is it? You are not missing other data?

BobCAD cannot help you with this?
I would think you would get a post working with your machine when you run one of their Software.

bert4255 said:

I'm trying to modify my post for a anilam 4200t cnc and when i post a program to do threads it gives me this

*TOOL #4 THREADING TOOL
T4
M41
G97 S600
G0 X1.17 Z.0575 M3
M8
G83 E0.0312 Z0.62 C0.01 D0.027 A60 S2
G0 X2. Z-.5625
G0 Z.1
M5
M2

I need the E to give me threads per inch instead of the decimal it is giving me.
If anyone could look at my post and tell me what i need to change to fix it I'd be greatful.

here is my post

2002. Program Block 2. Thread

PI = 3.141592653589793

ZLENGTH = LATHE_GetProfileStartZ() - LATHE_GetProfileEndZ()
XTAPER = LATHE_GetProfileStartX() - LATHE_GetProfileEndX()
LEAD = round(LATHE_GetThreadLead(), 4)
FIRSTPASS = LATHE_GetThreadFirstCut()
TDEPTH = cos((LATHE_GetAngleIn() / 2) * PI / 180) * LEAD
TANGLE = LATHE_GetAngleIn()
SKIMS = LATHE_GetFinishNumberOfCuts()
ZRETRACT = LATHE_GetRoughRetractAmount()
STARTS = 1

OUTSTRING = "'G83',"
OUTSTRING = OUTSTRING&"'E"&LEAD&"'"
OUTSTRING = OUTSTRING&"'Z"&Round(ZLENGTH, 4)&"'"
OUTSTRING = OUTSTRING&"'C"&Round(FIRSTPASS, 4)&"'"
OUTSTRING = OUTSTRING&"'D"&Round(TDEPTH, 4)&"'"
OUTSTRING = OUTSTRING&"'A"&Round(TANGLE, 4)&"'"
If SKIMS > 1 Then
OUTSTRING = OUTSTRING&"'S"&SKIMS&"'"
End If
OUTSTRING = OUTSTRING&"'R"&Round(ZRETRACT, 4)&"'"
OUTSTRING = OUTSTRING&"'X"&Round(XTAPER, 4)&"'"
OUTSTRING = OUTSTRING&"'W"&STARTS&"'"

CALL LATHE_ProcessPostLine(OUTSTRING)

Click to expand...

I'm not a bobcad user, but maybe try adding a new variable? (if those are your variables up top)

(after LEAD)
TPI = 1 / LEAD

and change

OUTSTRING = OUTSTRING&"'E"&TPI&"'"

Try at your own risk....

Alicante said:

Does not see the E section in your post.
Are you sure this is it? You are not missing other data?

BobCAD cannot help you with this?
I would think you would get a post working with your machine when you run one of their Software.

Click to expand...

The E part is in red in the post, It is for a canned cycle. if i use it without a canned cycle it screws up the threads. I usually put a canned cycle in manually. figured someone on here would know. I only use bobcad rarely and can't justify buying support if i'm only using bobcad 2 or 3 times a year.

thesidetalker said:

I'm not a bobcad user, but maybe try adding a new variable? (if those are your variables up top)

(after LEAD)
TPI = 1 / LEAD

and change

OUTSTRING = OUTSTRING&"'E"&TPI&"'"

Try at your own risk....

Click to expand...

This.. Looks like easy to edit and mess up until you get what you want

Rounding errors may become a problem....

Bert4255,

Change LEAD = round(LATHE_GetThreadLead(), 4) to Round((1/Lathe_GetThreadLead),4). This will give you the threads per inch. I am not certain why your entire threading cycle is scripted out, but from what I can see in the code, it is to get 1 value. If you have any issues changing the post, just let me know and I will do what I can to help.

SeanDa said:

Bert4255,

Change LEAD = round(LATHE_GetThreadLead(), 4) to Round((1/Lathe_GetThreadLead),4). This will give you the threads per inch. I am not certain why your entire threading cycle is scripted out, but from what I can see in the code, it is to get 1 value. If you have any issues changing the post, just let me know and I will do what I can to help.

Click to expand...

SeanDa, That fixed it. you have no idea how frustrating that was. Thanks

SeanDa said:

Bert4255,

Change LEAD = round(LATHE_GetThreadLead(), 4) to Round((1/Lathe_GetThreadLead),4). This will give you the threads per inch. I am not certain why your entire threading cycle is scripted out, but from what I can see in the code, it is to get 1 value. If you have any issues changing the post, just let me know and I will do what I can to help.

Click to expand...

SeanDa, I'm having trouble with the rest of the G83 canned cycle, It will not post correctly. would you look at it for me? [email protected]

bert4255 said:

SeanDa, I'm having trouble with the rest of the G83 canned cycle, It will not post correctly. would you look at it for me? [email protected]

Click to expand...

Can you describe the problem or is it the same problem?

I saw this thread yesterday but it looked like you got hooked up so I didn't look closely at your code.

RTM said:

Can you describe the problem or is it the same problem?

I saw this thread yesterday but it looked like you got hooked up so I didn't look closely at your code.

Click to expand...

Its a different problem, I've had been dealing with trying to get a good post from day one, had this software and machine for several years and it is always a post issue. I have to go through and put G0 X0. Z0. T0
M0 between tool changes. I can't just draw the part, tool path it and post. spend hours trying to get it to post right. guess that's because it's not a popular controller and machine. need a brand name to get a perfect post. the threads per inch is ok now but it is not posting the rest correctly. I get Error G83 compound approach will exceed length of thread. It doesn't post feeds either, it should post like this


*TOOL #3 THREADING TOOL 3
T3
M41
G97 S200
G0 X1.371 Z-.0009 M3
M8
G1 X1.371 F.01
G83 E18 Z-.625 C-.015 D-.038 A60 s2
G0 x3.0
G0 t0
M5
M2

It should have the z,c,d in negative values. when i post i get something like this

*TOOL #3 T3 THREADING TOOL
T3
M41
G97 S200
G0 X1.575 Z-3.5848 M3
M8
G83 E18 Z0.5402 C0.01 D15.5885 A60 S2
G0 X2. Z-4.125
G0 Z.1
M5

do you know how I can fix this?


2002. Program Block 2. Thread

PI = 3.141592653589793

ZLENGTH = LATHE_GetProfileStartZ() - LATHE_GetProfileEndZ()
XTAPER = LATHE_GetProfileStartX() - LATHE_GetProfileEndX()
LEAD = Round(1/Lathe_GetThreadLead(), 4)
FIRSTPASS = LATHE_GetThreadFirstCut()
TDEPTH = cos((LATHE_GetAngleIn() / 2) * PI / 180) * LEAD
TANGLE = LATHE_GetAngleIn()
SKIMS = LATHE_GetFinishNumberOfCuts()
ZRETRACT = LATHE_GetRoughRetractAmount()
STARTS = 1

OUTSTRING = "'G83',"
OUTSTRING = OUTSTRING&"'E"&LEAD&"'"
OUTSTRING = OUTSTRING&"'Z"&Round(ZLENGTH, 4)&"'"
OUTSTRING = OUTSTRING&"'C"&Round(FIRSTPASS, 4)&"'"
OUTSTRING = OUTSTRING&"'D"&Round(TDEPTH, 4)&"'"
OUTSTRING = OUTSTRING&"'A"&Round(TANGLE, 4)&"'"
If SKIMS > 1 Then
OUTSTRING = OUTSTRING&"'S"&SKIMS&"'"
End If



CALL LATHE_ProcessPostLine(OUTSTRING)

I think I see a way this could be done differently to make the problem a bit easier to solve but before we think about that it might get you going faster if I see the profile you are cutting and the parameters that were entered to get the code we're looking at. What version of BobCAD are you using and can you upload the .bbcd file? You will have to ZIP it first in order to upload.

If you can't upload the exact file (proprietary) make one up that just contains the threading cycle and preferably a few tool changes just to try to track down your tool change issue. You can reply to the forum with the code as it SHOULD read and we can go from there.

This was corrected for bert4255 and the threading cycle now functions correctly.