Continue to Site

Welcome to MCAD Central

Join our MCAD Central community forums, the largest resource for MCAD (Mechanical Computer-Aided Design) professionals, including files, forums, jobs, articles, calendar, and more.

Register Log in

4axis angle output

M

marker4x4

New member
Hi everyone, here comes another of my "brilliant" questions, haha

In this simple scenario - how to set the post to output let's say 90.0 and -90.0 instead of 90.0 and 270.0 ???
I've tried (I think) all combinations on the 4-Axis Rotary Table and Specs tabs and I can't get this thing to work
smiley19.gif
smiley19.gif
smiley19.gif


Thanks all,
 
OK, here we go. While in Pro manufacturing, on the top toolbar, select Applications, and NC Post Processor. When the Gpost window opens, select your post, and open OPT file.


When your Opt file opens, selectMachine tool type, if it is not already there. When this window opens, you will notice several tabs along the top.


Select the Prim. Rotable Table tab. In area, "Rotary Axis Type", make sure that the checkbox for "-n to +n = max departure of rotary" is selected.


Now select the Axes tab on the top. Select the "USE_REPOS for limit checking" checkbox. You will notice a "View settings" button. Select it.


Now you see another set of tabs at the top. Select the Feedrate motion tab, and select "Auto select opposite solution within limits". Select the Rapid motion tab and select "Auto select opposite solution within limits". Select theAxis limits tab for the axis your are trying to control. Select "linear range", and enter "-180" for minimum and "+180" for maximum.


Save your post and exit. This post should output 180 to -180 for this axis. If it doesn't, I can post a FIL macro, that along with a CL command from Proe, that will correct the problem.
 
Hi Allan,

I think I get your drift - it makes perfect sense, but I can't seem to find the View Settings button in here; I'm still on 2001 if that matters.
I've tried to run a sample file anyway with the setting you recommended and the Gpost complains about the "...REPOS macro not to be found..." and still spits out 270.0 deg. Hmmm... see if you can think of something, I appreciate it very much!


View attachment 2109
 
I forgot, the "alternate" selection only is available on a 5 axis post. Have you tried it with just the "REPOS" selected. If this doesn't work, tell me what axis you are trying to control, and I will post the FIL file for you.
 
Well, your solution works perfectly in 5-axis mode. I guess, I could use some macro to "eat" all the B codes since the machine is 4-axis only.

Otherwise, if you can think of some FIL macro that would help to get what I need in the 4-axis mode, that'd be great. I'm trying to keep A axis within -180.0 and +180.0 values.

Thanks Allan,
 
This FIL macro sends the tool to X20, Y20, Z20, and A0 without outputting the code to the tape file. To use this, you must add a CL command at the end of the NC sequence just prior to execution. The CL command is GOHOME / TABLE. Make sure to put the space before and after the "/".


View attachment 2110


You should also change the Rotary Axis Type to
 
appinmi said:
This FIL macro sends the tool to X20, Y20, Z20, and A0 without outputting the code to the tape file. To use this, you must add a CL command at the end of the NC sequence just prior to execution. The CL command is GOHOME / TABLE.
Click to expand...

Allan, do I need the GOHOME command at the end of every NC Sequence that uses any kind of rotary movement?
 
I have been doing a bit of reading, and I am going to write a "REPOS"macro to solve this problem. I could really use it with some of my posts, instead of trapping it with several other macros. I won't be able to work on it until late tomorrow or maybe even Friday. I will post my results when I get it done.
 
appinmi said:
I have been doing a bit of reading, and I am going to write a "REPOS"macro to solve this problem. I could really use it with some of my posts, instead of trapping it with several other macros. I won't be able to work on it until late tomorrow or maybe even Friday. I will post my results when I get it done.
Click to expand...

No hurry whatsoever - your help is much appreciated as it is
smiley1.gif
smiley1.gif


BTW: when the angle is set to -n<-->+n, and the Max. Departure is set for 180.0, the post should output anything between -180.0<-->180.0 right? But it does, and I don't know why. Am I missing something, or it's just the post?
 
It is just the post. The only way to get this to work, is to let it do a REPOS if it is out of limits. The 4 axis post doesn't have the ability to automatically fix this, I don't know why not, but can only look at a special macro to do this. That is what I am working on. The last upgrade for Gpost added the "auto" fix for 5 axis only.
 
Well, it wasn't as hard as I thought it would be. Just make sure that REPOS is active in your OPT file and the "A axis" limits are set to
 
Just to make sure, on the "machine Tool Type" window, in the "4 Axis Rotary Table" tab, "-n and +n" is checked. On the "Specs" tab, the "+/-0 outputs +/-0" is checked. On the "Axes" tab, "Use _REPOS for limit checking" is checked, and the limits for the A axis is set to -180 for minimum, +180 for maximum.
 
appinmi said:
You might want to see if your settings match this....
Click to expand...

Hmmm, I'm still having errors with the _REPOS macro - here's what it looks like (section of the .lst file):

......
68>GOTO /-13.586687,.900847,8.85296,-.995789,0,-.091675
68 68 Z12.7180$
71>CAMERA/0,0,1,0,0,1,0,0,-1,0,0,0
72>RAPID
73>GOTO /2.3168,4.337,9.2,1,0,0
73>ROTATE/AAXIS,STEP,179,CCLW
73 73 ***WARNING***
+&nbsp ;&nbsp ; INVALID MINOR WORD FOUND WITH ROTATE, IGNORED
73>RAPID
73>GOTO /2.3168,4.337,9.2,1,0,0
73 73 X-9.2000 Y4.3370 A-270.000$
73 73 Z2.3170$
73 73 ***WARNING***
+&nbsp ;&nbsp ; B-AXIS POSITION OUTSIDE LIMITS
74>CYCLE/DRILL,FEDTO,.15,IPM,25,CLEAR,.1
75>GOTO /2.2168,4.337,9.2,1,0,0
....

I'm at loss. Now, wouldn't be easier to convert this post to 5-axis, do the automatic repositioning (as you've suggesated in previous message) and just somehow supress the B (always on 0.0 anyway) output? Just a thought.
 
Wow Allan, this seem to work - you're DA MAN!

Oh, (I'm sure it's just a typo) - in the third line of your modified FIL macro it should read CURB not CURA
smiley1.gif
smiley1.gif


I owe you one - you ever go to Whistler for skiing??
 
You must log in or register to reply here.

Sponsor

Articles From 3DCAD World

Back
Top