ThreadC.dll

[Rocketmachinist]

Does anyone have any experience with threadc.dll. It is a simple G32 canned cycle that is used if you wanted to blend a series of threads together. Haas talks about it in their manual and the threadc.dll creates the tool path just fine but it screws up in posting. It post normal longhand threading cycles just fine. If you were to try and do the same thing with threadc.dll it gives an error when posting and doesn't give good code. It's a an easy program to write by hand.

 

[Guest]

4 minutes ago, Rocketmachinist said:

Does anyone have any experience with threadc.dll. It is a simple G32 canned cycle that is used if you wanted to blend a series of threads together. Haas talks about it in their manual and the threadc.dll creates the tool path just fine but it screws up in posting. It post normal longhand threading cycles just fine. If you were to try and do the same thing with threadc.dll it gives an error when posting and doesn't give good code. It's a an easy program to write by hand.

 

I saw a similar issue on Mastercam's website, If you encountered an issue with the product you might try contacting Cnc Software.

[Rocketmachinist]

17 hours ago, byte me said:

I saw a similar issue on Mastercam's website, If you encountered an issue with the product you might try contacting Cnc Software.

Yeah that was me and nobody responded. I did contact my reseller as well and they said I would have to get a custom post made for it. The toolpath posts but for some reason its all jumbled up. I don't really see how I can post a normal threading cycle under Longhand and get a G32 code to spit out and everything works fine. Then I try to do the same exact thing with threadc.dll and the people at Mastercam have no idea how it works. I will try to see if the mplmaster post works today. It is probably just an issue with the Generic Haas Post but I will try some different ones to see if they work instead. A G32 cycle is a G32 cycle. Threadc.dll just lets you do it as a chain.

[Rocketmachinist]

Ok i give up. I tried all the post on Mastercams website and they all give me the same error. It would be nice if they just added a contour feature into the new custom thread cycle. That one ran pretty awesome. The issue came up a couple of days ago because a guy on facebook was trying to thread an npt right into an nps. I showed him the page out of the Haas book and he might have been able to make the part. But the guy that taught me lathe told me that you can chain together G32 to follow an contour. He had used it in the past to make a nozzle for one of our facilities. It has 2 different sized Acme threads with the same pitch but were clocked to each other. He wrote the toolpath by hand and everything worked fine. For a normal G32 toolpath each line of the canned cycle only needs a few more points for it to work.

[Guest]

6 minutes ago, Rocketmachinist said:

Ok i give up. I tried all the post on Mastercams website and they all give me the same error. It would be nice if they just added a contour feature into the new custom thread cycle. That one ran pretty awesome. The issue came up a couple of days ago because a guy on facebook was trying to thread an npt right into an nps. I showed him the page out of the Haas book and he might have been able to make the part. But the guy that taught me lathe told me that you can chain together G32 to follow an contour. He had used it in the past to make a nozzle for one of our facilities. It has 2 different sized Acme threads with the same pitch but were clocked to each other. He wrote the toolpath by hand and everything worked fine. For a normal G32 toolpath each line of the canned cycle only needs a few more points for it to work.

The only information I could find on the topic is that it won't work with spline geometry.

[Rocketmachinist]

27 minutes ago, byte me said:

The only information I could find on the topic is that it won't work with spline geometry.

I'm just trying to get it to do a strait line right now and work from there.

Normal threading

 

Threadc.dll

 

This is the toolpath that I get from Mastercam with the normal threading cycle. It is the same minor diameter, major diameter, length of cut, feedrate. These two toolpaths should be identical.

O0000
(T)
(DATE=DD-MM-YY - 13-10-20 TIME=HH:MM - 06:12)
(MCX FILE - T)
(NC FILE - C:\USERS\ASMURPHY\DOCUMENTS\MY MASTERCAM 2021\MASTERCAM\LATH...\T.NC)
(MATERIAL - STEEL INCH - 1030 - 200 BHN)
G20
(TOOL - 97 OFFSET - 97)
(OD THREAD RIGHT  INSERT - NONE)
G00 T9797
M8
G97 S200 M3
G00 G54 Z.2435
X3.3836
X3.0775
G99 G32 Z-1.5048 E.08333
G00 X3.3836
Z.229
X3.0252
G32 Z-1.5048 E.08333
G00 X3.3836
Z.2178
X2.9848
G32 Z-1.5048 E.08333
G00 X3.3836
Z.2083
X2.9507
G32 Z-1.5048 E.08333
G00 X3.3836
Z.2
X2.9206
G32 Z-1.5048 E.08333
G00 X3.3836
Z.2
X2.9206
G32 Z-1.5048 E.08333
G00 X3.3836
Z.2435
M9
G53 X0.
G53 Z0.
M30
%

 

This is what i get using threadc.dll and keep in mind that mastercam is calling the same g32 cycle in the post. I checked that with the post debugger.

 

%
O0000
(THREAD C)
(DATE=DD-MM-YY - 13-10-20 TIME=HH:MM - 06:13)
(MCX FILE - T)
(NC FILE - C:\USERS\ASMURPHY\DOCUMENTS\MY MASTERCAM 2021\MASTERC...\THREAD C.NC)
(MATERIAL - STEEL INCH - 1030 - 200 BHN)
G20
(TOOL - 97 OFFSET - 97)
(OD THREAD RIGHT  INSERT - NONE)
G00 T9797
G97 S200 M3
G00 G54 Z.1216
X3.5206
G99 G01 X3.1836 E.08333
Z-1.5048
G00 X3.5206
Z.1035
G01 X3.1182
Z-1.5048
G00 X3.5206
Z.0895
G01 X3.0678
Z-1.5048
G00 X3.5206
Z.0777
G01 X3.0253
Z-1.5048
G00 X3.5206
Z.0673
G01 X2.9878
Z-1.5048
G00 X3.5206
Z.0579
G01 X2.9538
Z-1.5048
G00 X3.5206
Z.0493
G01 X2.9226
Z-1.5048
G00 X3.5206
Z.0487
G01 X2.9206
Z-1.5048
G00 X3.5206
Z.0487
G01 X2.9206
Z-1.5048
G00 X3.5206
Z.1216
X-1. Z-1.
G32 X.0003 Z0. E.08333
G00 X.2
X-1. Z-1.
G32 X.0006 Z0. E.08333
G00 X.2
X-1. Z-1.
G32 X.0008 Z0. E.08333
G00 X.2
X-1. Z-1.
G32 X.0011 Z0. E.08333
G00 X.2
X-1. Z-1.
G32 X.0014 Z0. E.08333
G00 X.2
X-1. Z-1.
G32 X.0017 Z0. E.08333
G00 X.2
X-1. Z-1.
G32 X.002 Z0. E.08333
G00 X.2
X-1. Z-1.
G32 X0. Z0. E.08333
G00 X.2
Z.037
X-1. Z-1.
G32 X0. Z0. E.08333
G00 X.2
X-1. Z-1.
G01 X.0234 Z0.
X-3.0096 E1.
M5
G00 G53 X0.
G53 Z0.
M30
%

 

[Zaffin_D]

The ‘C’ in threadC means contour, so using it with a single entity is not really it’s intended use.

Your reseller is correct, a custom post is required; I’m not aware of any CNC post that supports threadC.  This is because threadC writes it’s parameters to the NCI and doesn’t fill out the normal threading NCI lines.

[Rocketmachinist]

1 hour ago, Zaffin_D said:

The ‘C’ in threadC means contour, so using it with a single entity is not really it’s intended use.

I know its designed for contour threading. I use babysteps to make sure it can handle something simple before i get thrown in the deep end. I would love to see them just add those features to the custom thread cycle. I did some really cool stuff with that and it was super easy (see attached). Mastercam spent a lot of time developing this toolpath with the post that are already there. It just seems weird to me that they just kinda forgot about threading a contour when I can see using it more than rope threading.