| | |
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 .Originally Posted by jakemestre
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 ?
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
Last edited by jakemestre; 11-29-2011 at 08:51 PM.
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.
I have not tried it yet, but I think Tormach has a mastercam post on there
website.
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
Tormach PCNC1100, Mach 3 R3.043.037, MastercamX5 level 3.
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...
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.
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
Last edited by btu44; 11-30-2011 at 03:48 PM.
Tormach PCNC1100, Mach 3 R3.043.037, MastercamX5 level 3.
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...
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!
Posting Permissions
| | |
LinkBack URL
About LinkBacks
