Old school stuff

Hello,
I have an old supermax ycm 40 mill w/ a crusader m control and develop programs using mc v7 and have run it for years with no problem. I recently decided to try some thing new. I was wanting to pocket a hole using helix entry rather than ramping and supprise, the post put out arcs all the way around the hole and the plunged the Z axis to depth at the end of the cycle. When I turned off the arc command helix in entry, in the pocketing program it made linier moves with the Z movement on the same line, bout the same as ramping. The machine is capable of moving all three axis at the same time, because I can thread mill ID/OD threads with the control. I'm thinking it is in the post. When I run the fanuc post it produces the desired axis movement in the nc file. I have tried several things with my post but have ended up lacking the desired results. I was wondering if someone might have the time to look at my post and possibly give me some direction on what has eluded me? Thanks for your support. TOM

Put up the NC code

- I would guess the post that controls that aspect had not been proved correct to run on your machine

Some posts output a full arc, ( with comp applied ) with a Z move, you would expect it to work....but all it did was plunge
- you may have to break full arcs into 180° maximum sweeps.....
I seem to remember that V7 has a setting to NOT make(draw) full arcs at all

Try breaking the arcs into 2 pieces, re-chain them, and see what happens them, before doing any post mods

Thanks Superman,
I have tried breaking the into 90 degree quaderants, 180 , 360,. I've enabled/disabled full arcs, helix all axis, xy,xz, ect. support all arcs, with no luck. I'm just missing something. Here is what I have:Attachment 243568Attachment 243566 You might have to use notepad to open attachments. Tom

Putting your code up & marking the Z moves...
- it seems as if you may not be selecting the ramp options correctly

V7 is soooooo old, I forget how the layout was shown
- you should have an angle field that sets the helix pitch & and a helix radius ( try 45% of the cutter size & 1°-3° angle) ... and helix distance from profile ( set a small value)
- you should also have an option to center on a point ( helixes around this point, ie you may have a pre-drilled hole etc )
- there are other options, on what to do if the pocketing fails

Code:

---

%
N100G70G90
N102G29T1003X.5Z0
N104G90
N106G00
N108T0
N110Z0
N112M5
N114X-5.Y-5.
N116T03F24.4
N118M03
N120G00X.1961Y.0963
N122Z.1                            (Z move)
N124G03X-.1681Y-.0963I.014J0.
N126X.1961Y.0963I.014J0.
N128X-.1681Y-.0963I.014J0.
N130X.1961Y.0963I.014J0.
N132X-.1681Y-.0963I.014J0.
N134X.1961Y.0963I.014J0.
N136X-.1681Y-.0963I.014J0.
N138X.1961Y.0963I.014J0.
N140X-.192Y0.I.014J0.
N142G01X.0125Y0.Z-.2                            (Z move)
N144G03X-.0625Y0.I-.025J0.
N146X.1125Y0.I.025J0.
N148X-.1625Y0.I-.025J0.
N150X.2125Y0.I.025J0.
N152X-.0364Y.2372I-.025J0.
N154G01X.02Y.025
N156X.22Y.025
N158G03X0.Y.245I0.J.025
N160X-.245Y0.I0.J0.
N162X.245Y0.I0.J0.
N164X0.Y.245I0.J0.
N166X-.22Y.025I0.J.025
N168G01X-.02Y.025
N170X.02Y.03
N172X.22Y.03
N174G03X0.Y.25I0.J.03
N176X-.25Y0.I0.J0.
N178X.25Y0.I0.J0.
N180X0.Y.25I0.J0.
N182X-.22Y.03I0.J.03
N184G01X-.02Y.03
N186G00Z.1                            (Z move)
N188G0T0Z0
N190M5
N192X-5.Y-5.
N194G29E
%

---

currently your post is set to NOT break arcs, IJK values are absolute centers,
- not sure about helix_arc in ALL planes....your post only allows IJ output for any arcs meaning you can only work in G17....see "pcir"

it nearly looks as if your post is a V9 version thrown onto V7 software.... should post still, but hard to say...it is not good practice as some items defined in V9 may not have existed in V7.....so just to be aware

Code:

---

breakarcs : 0      #Break arcs, 0 = no, 1 = quadrants, 2 = 180deg. max arcs          2
arctype  : 1      # Arc center 1=abs, 2=inc, 3=st-cen, 4=unsigned inc.              1
do_full_arc : 1    #Allow full circle output? 0=no, 1=yes                          0
helix_arc  : 1    #Support helix arc output, 0=no, 1=all planes, 2=XY plane only  2

---

my suggestions are in blue

Superman,
Yes all my equipment and me are old. I worked for my father until he passed and they became mine.Tried your suggestions and to no avail. I'm thinking it might be in with the G02 and G03. As you can see it is putting out arcs, but not allowing Z outputs on the same line. Then one of the things we had done to the post was to break the post into sections for drip feeding large programs. Don't remember what the proxy statements do to the overall post config. I ran a fanuc post with the same test hole data and it posted fine (machine wouldn't except code). If anything else comes to mind let me know. Thanks

oops, just looked at your post again, ( your comment about no Z on arcs )......... it doesn't post any Z outputs on an arc

Your post

Code:

---

pcir        # Circular interpolation                                2
              pnmark, sgplane, sccomp, sgcode, pxy, i, j, pfr, pcan

---

Fanuc X5, 3 axis post

Code:

---

pcirout1        #Output to NC of circular interpolation
      pcan1, pbld, n$, `sgfeed, sgplane, sgcode, sgabsinc, pccdia,
        pxout, pyout, pzout, pcout, parc, feed, strcantext, scoolant, e$

---

notice the difference ie pxy is same as pxout & pyout combined, but there is no reference to a Z output in your postblock
- your post will only do planar movement on arcs

I would say linear ramp is your only option

I say that really sucks capability wise with what is considered normal practice with today's tooling

IMO, you may have to look thru your other posts that have the ramp on arc capability, & modify it to get the same code output....this will be difficult & a bit time consuming as you would have to post code & then prove it on your machine ( even if modified by someone else)

Thanks Superman,
With what you pointed out, I think I was able to solve the problem by simply telling the pcir code to put out pxy, z, i, j, the resulting code looked good initially I'll see when it hits the control. I'll let you know.

Quote:

---

Originally Posted by Superman

oops, just looked at your post again, ( your comment about no Z on arcs )......... it doesn't post any Z outputs on an arc

Your post

Code:

---

pcir        # Circular interpolation                                2
              pnmark, sgplane, sccomp, sgcode, pxy, i, j, pfr, pcan

---

Fanuc X5, 3 axis post

Code:

---

pcirout1        #Output to NC of circular interpolation
      pcan1, pbld, n$, `sgfeed, sgplane, sgcode, sgabsinc, pccdia,
        pxout, pyout, pzout, pcout, parc, feed, strcantext, scoolant, e$

---

notice the difference ie pxy is same as pxout & pyout combined, but there is no reference to a Z output in your postblock
- your post will only do planar movement on arcs

I would say linear ramp is your only option

I say that really sucks capability wise with what is considered normal practice with today's tooling

IMO, you may have to look thru your other posts that have the ramp on arc capability, & modify it to get the same code output....this will be difficult & a bit time consuming as you would have to post code & then prove it on your machine ( even if modified by someone else)

---

That is one way to do it, same as what it does for linear moves (prapid & plin )

if you placed it in the pxy postblock, to suit the statement in the revision log regarding non-modal outputs, but that would stuff prapid & plin & end up with double Z address outputs
I think you picked the right area