[Machineit]

I went into the debug mode and did not see an obvious entry to change, so here's the question.

How do I make the post not repeat the spindle speed on each and every operation with the same tool. There are times when that may make the speed posted 30 or 40 times within the same tool and making changes is nearly impossible.

Just want the speed posted when there is a change or at tool changes.

Thanks in advance------Mike

[A1CNC]

I would like to know that as well.

I was able to get mine to post a changed speed for the rough and finish tool but now it does the same as yours (posts spindle speed at each operation.)

[SeanDa]

Please put your post processor on here so I can review it

[Machineit]

Sorry, should have remembered to name it. It is just the standard Haas VF post.

Mike

[The Engine Guy]

Mike

Open the Post in Notepad and go to block 4 in the Post and remove the ",s" I`ve highlighted in Red and that should stop it outputting spindle speeds until the next tool change.

4. Null tool change
" "
"(NEXT CUT - SAME TOOL)"
system_comment
feature_name_comment
" "
n,rapid_move,force_x,xr,force_y,yr,rotary_xyr_angl e,,s
output_rotary_angle

Hope that works for you :-) :-) :-)

Regards
Rob
:rainfro::rainfro::rainfro:
.

[Machineit]

Mike

Open the Post in Notepad and go to block 4 in the Post and remove the ",s" I`ve highlighted in Red and that should stop it outputting spindle speeds until the next tool change.

4. Null tool change
" "
"(NEXT CUT - SAME TOOL)"
system_comment
feature_name_comment
" "
n,rapid_move,force_x,xr,force_y,yr,rotary_xyr_angl e,,s
output_rotary_angle

Hope that works for you :-) :-) :-)

Regards
Rob
:rainfro::rainfro::rainfro:
.

Thanks----I'll give it a go!

Mike

[Machineit]

Worked like a charm----You Da MAN!!!!!

Much Thanks and Cheers---Mike

[Machineit]

Another question for you, but I'll start another thread if necessary.

On my Haas and also my friends, the CAM tapping cycle does not work. Won't work with G99 G95 G94's etc. (feed/rev)

Any way other than manually entering it (as I do, but he can't) to get it to post as a simple RPM and feedrate, and not feed per revolution? If you use manual speed and feeds it will not change anything, because if you change the speed you also have to manually change the feed, so for someone like my friend, it does go good.

Example of current post:
T3 M06
G90 G54 X0. Y0. S2505 M03
G43 H3 Z0.1 M08
G95
G84 G99 X0. Y0. Z-0.7 R0.1 F0.05
G80
G94

Would like for example:
T3 M06
G90 G54 X0. Y0. S2505 M03
G43 H3 Z0.1 M08
G84 X0. Y0. Z-0.7 R0.1 F125.25
G80

Of course I would not normally post a spindle speed of S2505, but that was because the post processor was setting an even feed of F0.05

Thanks in advance for you time.

Cheers----Mike

[jvangelder]

check line 427


below is copied right out of my fanuc oimc post i use


427. Tapping feed rate (1=ipm 2=ipr)? 1


edit:

also check line 177

below is again out of my post
177. Tapping canned cycle.
rigid_tapping_start
n,g_canned_cycle,g98_g99,rotary_xy_f,rotary_xy_ang le,drill_depth,reference_plane,dwell,canned_feed_r ate

in your case, just use,

177. Tapping canned cycle.
rigid_tapping_start
n,g_canned_cycle,rotary_xy_f,rotary_xy_angle,drill _depth,reference_plane,dwell,canned_feed_rate


-Jacob

[Machineit]

Jacob,

Again, thanks for your help. I made the changes you mentioned then went ahead and did some experimenting.

On my Haas and others I believe the G94 and G95 prior and post the canned cycles are not needed or desired. To eliminate them, I deleted two lines completely, 22. and 23. That kept them from being posted. (see below)

[COLOR="Red"]22. Rigid tapping start.
n, "G95"
23. Rigid tapping end.
n, "G94"[/COLOR]

Then, instead of removing the "g98_g99" from just the tapping cycle, I removed it from all of the canned cycles. Now everything works great with no more invoking these unnecessary codes in my programs. It was easy to do, just went to "Edit" -- Replace. Typed in "g98_g99" to "replace" and left the "replace with" box empty.

For those who do not know, when you switch the tapping from IPR to IPM, it makes it easy to change your tapping stuff in the edit for the tapping tool. You already have the tap, for example 1/4-20, so when you go to manual instead of system settings, you can just change the RPM to whatever you feel comfortable with and when you post, the feed will be correct, as the pitch is already entered there. So, if you prefer to tap at a slower setting you can just enter that (like 500 RPM) or make it 5000 rpm if you like. The feed will stay correct.

I made quite a few other changes, trying to simplify some codes, but kept running into problems and had to change back. For example, to make the codes more like I like them, I wanted the location on the first hole in a canned cycle not to appear in the line with the canned cycle parameters. For example: G84 X.5 Y-1.4 Z-.5 R.1 F50. I wanted it just to read: G84 Z-.5 R.1 F50. That location is already in the previous lines of code.

To do this I removed the ",x_f,y_f" from the canned cycle line. Well, it no longer appeared in the line, but it would add a line after the cycle that had it move to X0. and Y0, which would add a hole there. To remove that I had to remove line #52 (I think it was). Okay, now it was done and posted it right. But, it no longer moved to the next hole if you had multiple holes to tap or drill. So I had to change that back. I really wished it had worked, because it wrote the code so much more simplified. I am one of those who watch the code as it runs to look for errors and it make it so much easier to follow. Old school I guess.

It is fun to play with the post. For those of you wanting to do it, make sure to save the original and copies in the various stages you try. It is much easier to go back if it is not good.

Anyway, thanks again and have fun all.

Mike

One last note. The post always put a rapid move the machine home (G91 G28) to the X, Y, and Z at the beginning of every program. I hated that and manually removed it from all of my programs. To fix that I went to line #2 and removed the following;

n,rapid_move,incremental_coord,"G28","Z0."
n,rapid_move,incremental_coord,"G28","X0.","Y0."

Now that is gone too.


"MAKE SURE YOU TEST ANYTHING YOU DO, I AM AND WILL NOT BE RESPONSIBLE!!!!!!!!!!!!!!!!"

Mike

[Machineit]

Well,

This does not seem to work. You must leave it on "System Auto" and change the percentage of the spindle to make adjustment for it work right. Otherwise you will need to enter the spindle speed and the feed rate in "Manual."

It's a work in progress at this point. I'll get right back to you on this.

Mike



For those who do not know, when you switch the tapping from IPR to IPM, it makes it easy to change your tapping stuff in the edit for the tapping tool. You already have the tap, for example 1/4-20, so when you go to manual instead of system settings, you can just change the RPM to whatever you feel comfortable with and when you post, the feed will be correct, as the pitch is already entered there. So, if you prefer to tap at a slower setting you can just enter that (like 500 RPM) or make it 5000 rpm if you like. The feed will stay correct.

[Joe S.]

If you do not like the idea of "deleting" the reference to g94, g95 you can comment them out in case you may need them for another machine in the future, ( g94) the round brackets will still allow them to print into your program, but they will show up as comments and have no effect upon the program.
my 2 cents!
BTW
Thank you all for this post, it prompted me to address these same issues. I noticed when I made these 2 changes the method of entering the feed rate changed where I used to set feed to 100 and rpm to tpi x 100 or some other multiplier, now I have to install feed as a decimal equal to 1/tpi, or as stated above use system automatic method,
both are good as long as I know what to do, it saves having to edit every program, and I am happy to exile the extra sRPM statements !
I added comments at the top of my post processor to explain the methodology used in setting the feed rate in case I am replaced by someone else too. Look out for the next guy, he just might be YOU !

[Joe S.]

One last note. The post always put a rapid move the machine home (G91 G28) to the X, Y, and Z at the beginning of every program. I hated that and manually removed it from all of my programs. To fix that I went to line #2 and removed the following;

n,rapid_move,incremental_coord,"G28","Z0."
n,rapid_move,incremental_coord,"G28","X0.","Y0."

Mike

Oh YEAH ! When I get time ! I build some tall fixtures and that has caused me some grief when an $80 cutter wipes out an $x,xxx fixture and itself too, big issue on my Fadal as it zeros in the table center.

[Machineit]

Oh YEAH ! When I get time ! I build some tall fixtures and that has caused me some grief when an $80 cutter wipes out an $x,xxx fixture and itself too, big issue on my Fadal as it zeros in the table center.

Ouch!!!!

Yah, don't understand that one at all. Used to startle the hell out of me!!