What's new
What's new

Brother Speedio Mastercam post help

Finegrain

Diamond
Joined
Sep 6, 2007
Location
Seattle, Washington
Hi guys,

I have a very old Mastercam post for my Speedio S700X1. It only emits J format G77 calls, like this:

G99G77Z-.5512R.03J31.75S2000

I would like it to us this format for metric threads:

G99G77Z-.5512R.03I0.8S2000

Sometimes the J format looks OK math-wise, like in the above case J31.75 is exactly the same as I0.8. However, I have some experience recently that makes me think that the control does not treat these the same way.

Anyway, I want my post to use I for metric and J for English. I have been hand-editing J's to I's for awhile, but sometimes I miss one, and it's also possible to make a typo and then have a bad day (I don't want to talk about it :wall: ).

Can someone show me the code in their post that switches to I format for metric threads?

Thanks, and regards.

Mike
 
I would try here;eMastercam Home

It's a tough thing, asking someone to "free brain" Edit your post processor Via an Internet forum, not all of us are named Bill. But it's really not that complicated once you see it. Do you know how to edit your post processor?

R

FYI fair warning. They run a tight ship over there.
 
What version of Mastercam are you using?
I personally have never seen the tap feed controlled by an I or a J, is this something that you've manually changed?
I can send you a snippet of my post but I doubt that would help you since my post uses IPR for all tap feedrates.
 
What version of Mastercam are you using?
I personally have never seen the tap feed controlled by an I or a J, is this something that you've manually changed?
I can send you a snippet of my post but I doubt that would help you since my post uses IPR for all tap feedrates.

Mastercam 2018
With my post, tap feeds are always emitted using J. The only changes I have to make are switching over to I for metric, and using G277 instead of G77 for peck tapping.

Regards.

Mike
 
It's a tough thing, asking someone to "free brain" Edit your post processor Via an Internet forum, not all of us are named Bill. But it's really not that complicated once you see it. Do you know how to edit your post processor?

Just want to look at some code samples. I can edit the post, maybe :crazy:. I just don't know what edits to make. It's been many years since I worked in SW development and that part of my brain was repurposed with speeds and feeds.

Regards.

Mike
 
Like I said it's a lot to ask over the Interphone.

1. Why are you using G77 instead of G84? >Snippet from the programming manual; "Set the data on a thread pitch following the address I, and the data on a number of threads following the address J"

2. Why are you using an "old post" if you have 2018 Mastercam? (You have paid for Maintenance, they have an entire support team waiting to help you, use it.) Unless........?

But if you really want to do it here; Edit/Open external/Open your post processor/Search G77 and all it's switches/Paste them here. I'll try and see what switches to change. But you really, really have the Carriage before the Horse here.

R
 
My post doesn't have a G77,so I really can't help you there.
It's very similar to a Fanuc post, maybe you can look at the default Fanuc post that comes with Mastercam?

This is what my Ptap part of the post looks like in my 2019 post:
Code:
ptap$            #Canned Tap Cycle
      pdrlcommonb
      result = newfs(17, feed)  # Set for tapping Feedrate format
      if met_tool$,
        [
        if toolismetric, pitch = n_tap_thds$  #Metric NC Code - Metric Tap
        else, pitch = (1/n_tap_thds$) * 25.4  #Metric NC Code - English Tap
        ]
      else,
        [
        if toolismetric, pitch = n_tap_thds$ * (1/25.4)  #English NC Code - Metric Tap
        else, pitch = 1/n_tap_thds$           #English NC Code - English Tap
        ]
      pitch = pitch * speed #Force Units Per Minute for regular Tap cycle
      #pbld, n$, sg94, e$
      pcan1, pbld, n$, *sgdrlref, *sgdrill, pxout, pyout, pfzout, pcout,
        prdrlout, *pitch, !feed, strcantext, e$
      pcom_movea
 
I use Inventor HSM and it spits this out:

G77 X75.075 Y-38.192 Z3.498 R35.488 P0 F1000

I have to manually change P0 to I0.8 and the F to S... every time I tap a hole. Apparently Inventor doesn't have a variable for metric pitch, so there's nothing the post processor can do. The upside is the machine stops if I forget to edit it vs. plowing through at some bad pitch. Inventor has a forum, I suppose mastercam does too. Local Yamazen dudes here say the local Mastercam dealers have a good speedio post, but I havent't switched cam programs.
 
2. Why are you using an "old post" if you have 2018 Mastercam? (You have paid for Maintenance, they have an entire support team waiting to help you, use it.) Unless........?

1. Posts are a separate revenue source for Mastercam resellers, and their price for a Speedio post was not a small amount of $$.
2. When I said I might want one, they said, "What's a Brother Speedio?" I had very low confidence they would provide a post that worked right away, and I did not want to be their test bed.

Regards.

Mike
 
I use Inventor HSM and it spits this out:

G77 X75.075 Y-38.192 Z3.498 R35.488 P0 F1000

I have to manually change P0 to I0.8 and the F to S... every time I tap a hole. Apparently Inventor doesn't have a variable for metric pitch, so there's nothing the post processor can do. The upside is the machine stops if I forget to edit it vs. plowing through at some bad pitch. Inventor has a forum, I suppose mastercam does too. Local Yamazen dudes here say the local Mastercam dealers have a good speedio post, but I havent't switched cam programs.

Are you on the latest Speedio post?
 
Local Yamazen dudes here say the local Mastercam dealers have a good speedio post, but I havent't switched cam programs.

Yes, I was told that as well, but it was a different region's Mastercam reseller that had the Speedio post, and apparently they don't share stuff like that, so my region's reseller was only able to offer to write one from scratch for a lot of $$.

Regards.

Mike
 
Yes, I was told that as well, but it was a different region's Mastercam reseller that had the Speedio post, and apparently they don't share stuff like that, so my region's reseller was only able to offer to write one from scratch for a lot of $$.

Regards.

Mike

That's a crock of shit if they were going to charge you. If you're on maintenance simple 3 axis posts are no charge. The posts they charge for are 5ax
 
1. Posts are a separate revenue source for Mastercam resellers, and their price for a Speedio post was not a small amount of $$.
2. When I said I might want one, they said, "What's a Brother Speedio?" I had very low confidence they would provide a post that worked right away, and I did not want to be their test bed.

Regards.

Mike

I've been through it trust me. Notice in most of my posts about Mcam I call it Mastersuk. BUT in my experience you just need to tighten the wrench. They have a tiered support system, meaning the more assertive you are the higher up on the tier you get. The initial person may as well work at McDonalds.

This is how it works. If you tell them you need a post for your machine, they tell you it'll cost $XXX.XXX, because that's what they want. They want to build you a custom post, that's big money. Shit if every Mcam user got a custom post.....$$$$

But you have Maintenance, so you need to be Assertive, which is another word for something else. And tell them You want the post you got with the Suite to work for you, after that, usually (which is another word for something else) the local guy will come into your office and ask you what you want and he'll do it for you. BUT now you're in it, you're involved, you're one of the guys. Just keep at them. Trust me, there is a working post for your Machine...you just need to find it, or make CNC-Sofware find it for you. Like Dew said though, it's part of the Maintenance package.
 
Yes, I was told that as well, but it was a different region's Mastercam reseller that had the Speedio post, and apparently they don't share stuff like that, so my region's reseller was only able to offer to write one from scratch for a lot of $$.

maybe your local Yamazen has a post they'd share? I think that was the case here.

Are you on the latest Speedio post?

No. I downloaded the HSM library one when I got my machine and have made a couple tweaks (with help from Inventor forum [FredS of here/there is awesome]). I know there is a fancier one out there, but mine's not broke, so I don't want to fix it. My understanding is the tap issue was Inventor and not post processor. I should mention I live in a cave. I got Inventor perpetual license in 2016 and I use HSM Xpress (2016). I don't pay rent on my software so I'm not in any hurry to change. I just managed to get my shop PC setup duplicated at home (legally) so cave is feeling fairly cozy.
 
My machine has the A00 control and I am using Solidworks CAM (which is CAMWORKS) and it has the same problem. My post is spitting out J's for metric pitches and using 5-6 significant figures and it is working well. Sample line shown below for M4x0.7. I pm'd this to Finegrain but thought I would toss it out in this thread.

G77 G98 R.7012 Z-.0988 Q0.0 J36.2857 S2500
 
Some might call this a work around/hack, but why not just convert your metric taps to inch and then they would post ok? In Mastercam I have metric taps saved as all inch dims. Same thing with endmills FWIW, 10mm=.3937 in my tool library, etc.
 
No. I downloaded the HSM library one when I got my machine and have made a couple tweaks (with help from Inventor forum [FredS of here/there is awesome]). I know there is a fancier one out there, but mine's not broke, so I don't want to fix it. My understanding is the tap issue was Inventor and not post processor. I should mention I live in a cave. I got Inventor perpetual license in 2016 and I use HSM Xpress (2016). I don't pay rent on my software so I'm not in any hurry to change. I just managed to get my shop PC setup duplicated at home (legally) so cave is feeling fairly cozy.

Well, the new Speedio post that HSM/Fusion CAM use now does proper tapping. For inch taps, it grabs the pitch from the tool library and converts it into TPI for the proper J argument automatically. It does all the other Speedio stuff as well (integrated probing, M400/M401 washdown, G100 tool changes, degree per minute 4th axis soon, etc). It isn't fully dialed in for some of the nitpicky go-fast stuff yet, but what is there is generally well tested.

This has nothing to do with subscription- all the latest posts are free.
 
Some might call this a work around/hack, but why not just convert your metric taps to inch and then they would post ok? In Mastercam I have metric taps saved as all inch dims. Same thing with endmills FWIW, 10mm=.3937 in my tool library, etc.

I'm not aware of a way in MCAM 2018 to say "this is a metric tool". When I define a tap, it asks me how many threads per inch. I don't see any checkbox or toggle that would let me define it as metric.

I can switch the entire config over to metric, but then I have the opposite issue with inch taps.

Regards.

Mike
 
I'm not aware of a way in MCAM 2018 to say "this is a metric tool". When I define a tap, it asks me how many threads per inch. I don't see any checkbox or toggle that would let me define it as metric.

I can switch the entire config over to metric, but then I have the opposite issue with inch taps.

Regards.

Mike

He means, in the field that you enter the Pitch. If its a 1mm pitch, in that field enter .03947 not 1.

R
 
Well, the new Speedio post that HSM/Fusion CAM use now does proper tapping. For inch taps, it grabs the pitch from the tool library and converts it into TPI for the proper J argument automatically. It does all the other Speedio stuff as well (integrated probing, M400/M401 washdown, G100 tool changes, degree per minute 4th axis soon, etc). It isn't fully dialed in for some of the nitpicky go-fast stuff yet, but what is there is generally well tested.

This has nothing to do with subscription- all the latest posts are free.

You mean this one? (search Speedio): Post Library for Fusion 36 and Autodesk HSM | Autodesk HSM

So, it taps metric threads with a J?

I work in all metric, I suppose that doesn't matter. I'll give a try sometime. Thanks. Sorry for the OT Finegrain
 








 
Back
Top