[jakemestre]

I was wondering if anyone on this forum is using Mastercam and has a good way to utilize metric taps in the Tormach tension/compression tapping head. When there are only a couple of holes it's one of those operations that takes as much time to tap by hand as to write the code by hand. If anyone out there could give a good description of how you do it, or even a short video that would be wonderful. Thanks in advance.
Jake Mestre

[hall6ppc]

I was wondering if anyone on this forum is using Mastercam and has a good way to utilize metric taps in the Tormach tension/compression tapping head. When there are only a couple of holes it's one of those operations that takes as much time to tap by hand as to write the code by hand. If anyone out there could give a good description of how you do it, or even a short video that would be wonderful. Thanks in advance.
Jake Mestre

I use Mastercam x3 with the Tormach . Have not done tapping with the tension/compression head though. I have edited my post a lot but getting it to post code when doing tapping would take a bunch of work ( not sure I could get it to work) . I can send you a the post if you like and you can give it a try . Just PM me .

[Freddy Bastard]

I can help you on this but I need some information.

What version of mastercam are you using?

What post are you using?

I've done a Mastercam post for Tormach (mpmaster_tormach) and it's on the yahoo tormach group.

On my latest post, I've added the T/C cycle.

To use a metric tap in a inch config, you'll have to create a new tap and you'll have to convert it's dimensions to inch. ie: a M5 X .8 tap, the diameter will be .1968'' and the number of thread per inch will be 31.75 with this, Mastercam will output the right feed/speed

[hall6ppc]

I can help you on this but I need some information.

What version of mastercam are you using?

What post are you using?

I've done a Mastercam post for Tormach (mpmaster_tormach) and it's on the yahoo tormach group.

On my latest post, I've added the T/C cycle.

To use a metric tap in a inch config, you'll have to create a new tap and you'll have to convert it's dimensions to inch. ie: a M5 X .8 tap, the diameter will be .1968'' and the number of thread per inch will be 31.75 with this, Mastercam will output the right feed/speed

Is you lastest post with the tapping added on the Yahoo Tormach group and can it be down loaded ?

[jakemestre]

Freddy Bastard,
Thank you very much for the info. I'm working with Mastercam X4 and needed exactly the advice you gave. It was the conversion that I wasn't taking into account, which was manifesting in some really big numbers in the post. I had actually just left the yahoo group a week ago and I'm not sure why. So join request in, and when that's approved I'll head over to download your PCNC Post. I'll probably have a question or two when I'm able to take a look at the output code. Which file would it be in at the group site? Thank you again.
Jake Mestre

[Freddy Bastard]

Ok, I'll have to take a look at this. The problem is that X4 is no more installed on my pc so I'll have to install it back to test and update the post.

If some of you are on X5, I've uploaded the latest post and machine file on the yahoo group. Older posts don't have the T/C logic in it.

[Ironman2525]

I have not tried it yet, but I think Tormach has a mastercam post on there
website.

[btu44]

Ok, I'll have to take a look at this. The problem is that X4 is no more installed on my pc so I'll have to install it back to test and update the post.

If some of you are on X5, I've uploaded the latest post and machine file on the yahoo group. Older posts don't have the T/C logic in it.

As I fully expected, the X5 post will not work on X3, but it was worth a try.

Freddy, would you be willing to explain briefly how you learned to edit MC posts. I can't find a thing about it on the internet, book or training.
All I've heard is it is good to know C++.
Much appreciated,
Barry

[Freddy Bastard]

Well, that's a big question. I've worked for a Mastercam reseller and it was part of my job to edit posts for customers. I started in V7 of Mastercam, got some post trainning at the Mastercam headquarter and a lot of learning by myself (there was a post guide in the Mastercam's documentation). Your reseller should have it (:
So if I understand well, some of you are on X3 and X4. I'll try to update the x3 and x4 posts in my lost time...

[btu44]

I have looked through the X3 Post Reference Guide and the various tutorial videos Mastercam has. I guess I need a Mastercam Posts for Dummies book.:withstupi

But I did try comparing your X3 post to the new X5 post. I did some copy and pasting of some likely entries. Like all entries below the [CTRL_MILL|MPMASTER_TORMACH] line and also the “soft tap” lines.
Hope you don’t mind?

Attached is a screen capture of the results

And here is the generated code:

(T265 - 1/2-13 TAPRH - H265 - D265 - D0.5000")
N100 G00 G17 G20 G40 G80 G90
N101 M998 ( TOOLCHANGE )
N102 T265 M06 ( 1/2-13 TAPRH)
N103 (MAX - Z1.)
N104 (MIN - Z-1.)
N105 G00 G90 G54 X0. Y0. S534 M03
N106 G43 H265 Z1.
N107 G94
N108 G98 G84 Z-1. R.1 F41.14
N109 G80
N110 G00 G90
N111 M05
N112 M998 ( TOOLCHANGE )
N113 G28 Y0.
N114 G90
N115 M30

I see there is no dwell or up and down feed rates changes. Also the Mach3 User Guide mentions that G84 is not supported. Just for fun I ran it as is on the Tormach and it actually worked as expected. But with out the dwell it looks like my T/C head would need a good 3” travel.
Also it looks like G84 does not support dwell anyways.
Does your Tormach have spindle RPM sensor?

So I was wondering if I’m getting close?
Does the “soft tap” entry reference something like a Chook?


Thanks Freddy

[Freddy Bastard]

Nope, I dont' use G84 for tapping. There's some more editing to do... The only thing you changed is the text area (text you'll see in Mastercam) but it won't change the nc output.

Hummm, I think soft tap refer to some test I did in the past, so it's not used.

Tomorrow in the morning, I'll try to install X3 and X4 and update the posts...

[Freddy Bastard]

Ok, here we go. It's done.
X3 and X4 posts are on the yahoo group in the file section. I've added a little doc on how to use it (don't know if I forgot something...)

Don't wait to long to test it because I'll uninstall my X3 and X4 version in a couple of days...

copy .MMD and .control file in the cnc_machines folder
copy the .PST file in the mill*---posts folder

Enjoy!

[btu44]

Thanks Freddy, this is way cool of you. :cheers:

I'll try them today.

Last night I spent time trying to figure out the X3 post again. I think I got it but I'll still your files.

N100 G00 G17 G20 G40 G80 G90
N110 M998 ( TOOLCHANGE )
N120 T200 M06 ( 1/2-13 TAPRH)
N130 (MAX - Z1.)
N140 (MIN - Z-1.)
N150 G00 G90 G54 X0. Y0. S247 M03
N160 G43 H200 Z1.
N170 G94
N180 S247 M3
N190 G01 Z-1. F19.
N200 M4
N210 G04 P.3
N220 G01 Z.1 F19.95
N230 G80
N240 G00 G90
N250 M05
N260 M998 ( TOOLCHANGE )
N270 G28 Y0.
N280 G90
N290 M30

[btu44]

I downloaded the post files and the Post Guide...much appreciated.

Here is some code using the X3 post. First toolpath is a cutter comp test and then a TC tap cycle.
The tap cycle looks good but the plunge rate for cutter comp looks like it would cause sphincter contractions...it should be 40 IPM.

I hate to turn this into some thing you'll regret but can this be fixed?

N100 G00 G17 G20 G40 G80 G90 G64
/ N110 M998 ( TOOLCHANGE )
N120 (CUTTER COMP)
N130 T200 M06 ( 1/2 FLAT ENDMILL)
N140 (MAX - Z1.)
N150 (MIN - Z-1.)
N160 G00 G90 G56 X1.88 Y.255 S2000 M03
N170 G43 H200 Z1. T201
N180 G00 G90 Z.1
N190 G94 G01 Z-1. F999999. (PLUNGE FEED)
N200 G41 D200 X1.505
N210 G03 X1.25 Y0. I0. J-.255
N220 G02 X-1.25 I-1.25 J0.
N230 X1.25 I1.25 J0.
N240 G01 G40 Y-.375
N250 G00 G90 Z1.
N260 M05
/ N270 M998 ( TOOLCHANGE )
N280 M01
N290 (TC TAP 1/2-13)
N300 T201 M06 ( 1/2-13 TAPRH)
N310 (MAX - Z1.)
N320 (MIN - Z-1.)
N330 G00 G90 G56 X0. Y0. S260 M03
N340 G43 H201 Z1. T200
N350 G94
N360 S260 M3
N370 G01 Z-1. F20.
N380 M4
N390 G04 P.3
N400 G01 Z.1 F20.
N410 G00 G90 Z1.
N420 M05
/ N430 M998 ( TOOLCHANGE )
/ N440 G28 Y0.
N450 G90
N460 M30

[Freddy Bastard]

Ho! that's a old bug!

I'll have to scatch my head to find what was the solution to this bug. If I remember, it was not really post related...
I'll take a look at this tomorrow, but I know for sure that there's a solution for this.

[btu44]

Speaking for myself don't sweat it. The copy and paste of your X5 post to the older X3 post is making good code for me. I'm just amazed you can figure this stuff out. I can know see why my dealer never responded to my post modification requests.
Again, thanks for putting your hard efforts out for us to use for free.

[Freddy Bastard]

Found the problem,X3 post is now corrected and uploaded on the yahoo group.

[btu44]

Spent yesterday running several programs with variety of toolpaths using the new post. Makes good code...thanks again.
And the M00's at each Tap Position is an added bonus.

[jakemestre]

Freddy,
Thank you so much for posting these files. Obviously there was a lot of effort that went into creating the files for each Mastercam version, and the one that I've seen is very well done. It's solved several things I've had difficulty with since day 1 of using my mill. Again thank you, and if there's anything I can do in return feel free to PM me.
Jake Mestre