[pejaer]

Hi all,

I have a 1100 and I am using a post processor for HSM works from Next Gen (I probably got it from this forum a few years ago).....I am not a power user...(i.e. could be that I am making a mistake)....but I have been experimenting with the "force tool change" or "measure tool" in the Manual NC option and neither of these seem to do anything. What I really want to do is raise and stop the spindle, flip my part, and start again AND in one Job/post. My work around is what I always have been doing and made 2 jobs with 2 posts. Seems like the function is there in HSMWorks, but perhaps the post does not handle these options? Any insight is appreciated. I did not check to see if others like "dwell" or "stop" work as I think they would not help my situation anyway.

Paul

PS I see in my title I listed myself as a SprutCam user....I shelved that some time ago and have been having much more success with HSM Works.

[hayes]

Seems like this would be very simple to hand code in the part program. After the work is completed with the last tool for Side1, put in something like this

G91 G28 Z0
G90
M1

Change part to Side2 and hit program start. There is also an HSM Works / HSM Express sub-forum here on the zone, you'll probably find much more knowledgeable input there.

[mountaindew]

I admit I use sprut and use auxiliary operation and set these codes in that operation.

Example pasted from sprut g-code

(Set g55 Workspace 0 x,y,z)
N5520 G55
N5530 G52 X0. Y0. Z0.
N5540 T1 G43 H1 M6
N5550 M1


g55 sets new offsets
g52 zeros out everything so when I touch off with t1 in next op it sets xyz correctly for the current g54,g55,g56 ........;
T1 is my hamier probe and that tells Me to touch off new coordinate system.
Then I hit alt r or run and it continues with asking for next tool and operations on that side or offset.
I do multi sided parts this way and find no reason to split the code and have even more files to manage ! Up to 6 g-code files per part can add up to hundreds of files to track after a while.

Note: there are a number of ways to do this. I found this works best for me


Throw in a clip of a multi side part with most the the operations listed note each ao for g54,g55,g56....
Attachment 272688
md

[SCzEngrgGroup]

Hi all,

I have a 1100 and I am using a post processor for HSM works from Next Gen (I probably got it from this forum a few years ago).....I am not a power user...(i.e. could be that I am making a mistake)....but I have been experimenting with the "force tool change" or "measure tool" in the Manual NC option and neither of these seem to do anything. What I really want to do is raise and stop the spindle, flip my part, and start again AND in one Job/post. My work around is what I always have been doing and made 2 jobs with 2 posts. Seems like the function is there in HSMWorks, but perhaps the post does not handle these options? Any insight is appreciated. I did not check to see if others like "dwell" or "stop" work as I think they would not help my situation anyway.

Paul

PS I see in my title I listed myself as a SprutCam user....I shelved that some time ago and have been having much more success with HSM Works.

HSMXpress will easily handle multiple fixtures in a single file. Put each in its own "job" folder, and set a different fixture number for each (0 for G54, 1 gor G55, etc.). The POST *should* respect that, and output the fixture selects (G54-G59) at the appropriate places in the g-code. I do this all the time, and use 3-4 fixtures in some jobs.

Regards,
Ray L.

[wtopace]

I admit I use sprut and use auxiliary operation and set these codes in that operation.

Example pasted from sprut g-code

(Set g55 Workspace 0 x,y,z)
N5520 G55
N5530 G52 X0. Y0. Z0.
N5540 T1 G43 H1 M6
N5550 M1


g55 sets new offsets
g52 zeros out everything so when I touch off with t1 in next op it sets xyz correctly for the current g54,g55,g56 ........;
T1 is my hamier probe and that tells Me to touch off new coordinate system.
Then I hit alt r or run and it continues with asking for next tool and operations on that side or offset.
I do multi sided parts this way and find no reason to split the code and have even more files to manage ! Up to 6 g-code files per part can add up to hundreds of files to track after a while.

Note: there are a number of ways to do this. I found this works best for me


Throw in a clip of a multi side part with most the the operations listed note each ao for g54,g55,g56....
Attachment 272688
md

THANK YOU! I have been looking for a simplistic write-up on this for a while now. I really like the auxiliary operation combined with the multiple work offsets. I will try this on my part that I finally gave up on and split out to multiple files.

Side note - how do you handle fixturing (for example: clamping the turner's cube in a vise) when doing a part like this?

[smokediver576]

I admit I use sprut and use auxiliary operation and set these codes in that operation.

Example pasted from sprut g-code

(Set g55 Workspace 0 x,y,z)
N5520 G55
N5530 G52 X0. Y0. Z0.
N5540 T1 G43 H1 M6
N5550 M1


g55 sets new offsets
g52 zeros out everything so when I touch off with t1 in next op it sets xyz correctly for the current g54,g55,g56 ........;
T1 is my hamier probe and that tells Me to touch off new coordinate system.
Then I hit alt r or run and it continues with asking for next tool and operations on that side or offset.
I do multi sided parts this way and find no reason to split the code and have even more files to manage ! Up to 6 g-code files per part can add up to hundreds of files to track after a while.

Note: there are a number of ways to do this. I found this works best for me


Throw in a clip of a multi side part with most the the operations listed note each ao for g54,g55,g56....
Attachment 272688
md

I would love to see a video of this part (Turner's cube) being machined. Maybe something like a 4 part video..... Cm'on, someone with more grey matter post something up!

*** update - sorry guys, now I feel pretty stupid now that I searched for it in YouTube! Maybe someone doing it on the Tormach.... ***

Later,
Awall

[mountaindew]

Hey smokediver576!
They are kind of boring to make, mostly turning big aluminum into little aluminum. Not shown in above clips the final one used to mill parts has 4 holes drilled and threaded on each side in corners. shown below.
Attachment 272732

Did this because I like to tap stuff with tc unit and its not hard to change tools and or design and add more detail or operations just to be silly or because you can.


Attachment 272730
Note the side is milled out because my test material/ stock was undersize of design and I expected this when I milled it

I Looked and don't have any uploaded clips of this in aluminum , will fix that.
md

[pejaer]

Hi Ray,

I have the edit feature open for my first "job" and I see a drop-down for "fixture" where I can select a body from my model, but I do not see a way to assign a number...can you elaborate where to make this assignment? Also, I am curious how HSMworks makes 1 G-code file from the 2 jobs...obviously you figured this out....but up to now, I can only get 1 job per 1 post g-code file.

Thanks
Paul

[SCzEngrgGroup]

Hi Ray,

I have the edit feature open for my first "job" and I see a drop-down for "fixture" where I can select a body from my model, but I do not see a way to assign a number...can you elaborate where to make this assignment? Also, I am curious how HSMworks makes 1 G-code file from the 2 jobs...obviously you figured this out....but up to now, I can only get 1 job per 1 post g-code file.

Thanks
Paul

Select the job, right-click, and select Edit, scroll down to the bottom, in the "Post Processing" section, set Work Offset. 0 = G54, 1 = G55, etc.

To output multiple jobs, select them (Click on the first, Ctrl-Click to select the others), then click Post Process. Check the g-code to make sure the G54, G55, etc are there. If not, then your POST needs a minor edit.

Regards,
Ray L.

[pejaer]

Hi Ray,

I think it might be a post process issue. I assigned the first job "0" and the second job "1" (typing in "0=G54" did not work, so I assume you did not mean this).....and I did the CTL-Select trick...(thanks for that easy one.....I did not know that was possible...!) and I see now both jobs in the Gcode, but it looks like just the G054 is in the code one time and no G055.

Paul

[SCzEngrgGroup]

Hi Ray,

I think it might be a post process issue. I assigned the first job "0" and the second job "1" (typing in "0=G54" did not work, so I assume you did not mean this).....and I did the CTL-Select trick...(thanks for that easy one.....I did not know that was possible...!) and I see now both jobs in the Gcode, but it looks like just the G054 is in the code one time and no G055.

Paul

Paul,

Upload your POST, and I'll take a look at it. You can find the path to it in the dialog where you select which POST you're using.

Regards,
Ray L.

[pejaer]

Hi Ray,

Thanks for your time, I appreciate it.....

I attached a zip file of my parts....if you want to look at these, make sure you use the assembly file ("machining setup") for our discussion. The post process file is attached. I needed to trick the upload function by changing the extension on the file name to ".txt". You might need to change this back to ".cps".

If you are looking at into it...and have this expertise....whereas your solution is good (maybe best?) I originally thought that simply adding a "manual NC" to force a tool change would be the way to go....you might look to see if that is an easier solution from a post process file change standpoint.

Paul

[SCzEngrgGroup]

Paul,

I have to say, that is, by FAR, the lamest HSMXpress POST I've ever seen....

In any case, I've modified it so fixtures work correctly. It never made sense to me for 0 ==> G54, so I've modified it so you put the actual fixture number in the Job->Edit dialog. For G54, put "54", for G55, put "55".

Not at all clear what you're wanting on the toolchange....

Regards,
Ray L.

[pejaer]

Hi Ray,

Thanks....I'll try this. And, if you know any better, I would certainly try it. I am sure I got this Post from this forum, and there is probably better ones for sure.

For the "tool change"....there is an option called "Manual NC"....right-click any job, scroll to "New Operation" then "Manual NC"....I was just looking for any option that would stop and raise the spindle to flip my part. If I understand it correctly, inserting this manual op in the job would do the trick. It is just that my Post (I assume) does not recognize these Manual NC functions.

Maybe the easier path is, as you hinted, look for a more sophisticated Post for the Tormach.

Paul

[SCzEngrgGroup]

Paul,

Ask on the Tormach forum for a copy of my personal POST modified for Tormach. Several guys there have versions of it.

Regards,
Ray L.

[pejaer]

Hi all,

In addition to the tips from you all, I stumbled on a likely solution/work around to my issue....this is something that everyone knows already except me.....but I thought I'd throw it out for others. In my case, I am using a .5" EM on the top and then want to use the same .5" EM after flipping the part....and I needed to therefore put in a pause to do the flipping. In my original program, I used the same EM (I should say "copied") the same EM for all my .5" Ops and it has the same tool assignment number, i.e. #1. If I simply go to my tool library and select the same EM from the library, HSMWorks assigns this same EM as #2. Although I did not mill a part yet, it looks like from the G code, the program will ask me for tool #2, which I will ignore but will allow me to flip the part.

Paul