[John F]

OK you seasoned users,

I am a new user of XP production and am trying to configure my post processor. None of the supplied posts work for our machines. We use Heidenhiem mill plus and a Seimens 432. I've tried the supplied post processors and had no luck.

I have created our own but in drilling cycles the peck depths come out in absolute. What I want is a canned cycle

ie G83 Y2 Z-27 B20 I3 K10 F.. S...

where Y Retract plane
Z final depth
B initial plane
K peck depth
not

N68 (5.8 DRILL)
N69 T1 G43 H1 D1
N70 M66
N71 F95.493 S823
N72 M03
N73 M08
N74 G00 X-39.82 Y36.512 Z25.
N75 Z0.5
N76 G01 Z-1.364 F47.746
N77 G00 Z0.5
N78 G01 Z-3.227
N79 G00 Z0.5
N80 G01 Z-5.091
N81 G00 Z0.5
N82 G01 Z-6.955
N83 G00 Z0.5
N84 G01 Z-8.818

Is there a switch or does it have to be defined in each G code unde posting format. If so how is this done? It has to be soo simple but this is eluding me.


John

[HuFlungDung]

Hi John,

No, there is no magic switch (I wish there were) for switching the values from absolute to incremental.

I was in a similar situation with my Shadow (Bandit type) controller, where the canned cycle amounts are always deemed to be incremental.

Here is the gist of what I learned: first, in order to make the simulation work accurately, you need to fill in those first boxes in the "Set clearances" field with, as you know, absolute values.

Next dialog is the "Select a cycle" dialog where you can pick your machine cycles. Note: there will not be any fields to fill in here if you did not associate some variables in "NC setup" canned cycle with the cycle in question.

So, you need to go to NC setup/Posting Format/add cycle (if you haven't already), then select a particular cycle to work on. Now, you can mess around with the default variables from the list of "Insert and Substitutions" if you like, but I think that absolute values are still the rule there. So, click "Add" to create a new variable. You can rename it to whatever is meaningful, instead of using the default name "parmater No 8" or whatever.

Then, set up your canned cycle using these custom variable names.

You can create as many as you need to fill in each parameter of your drill cycle. These new variables will be "stand alone" and they will show up in the NC canned cycle wizard in the "Select a cycle field". These values that you insert now, will be retained exactly as entered, and will be used to fill in your cycle values.

Take note: altering your canned cycle setup will cause problems when opening older files made with the canned cycle set up in a different fashion. One method to avoid this, is to create this new cycle setup under a new and unique Post name, leaving your old post as is.

This gets cumbersome to keep track of, so I simply "bite the bullet" and change it anyway. Whenever I open an old file containing drilling cycles, I simply delete all the cycles and do them again. If I still get a crash, then I delete the file in settings called NCGlobal_inch.bin, or if you work in metric, I suppose it would be NCGlobal_mm.bin. This contains your list of variable choices you have used in previous sessions. This is where the corruption occurs if you add new things to your nc cycles, because the new cycle cannot reconcile with the old. This is an active, temporary file, and is harmless to delete. However, you will note that you have to start over with tool and material selections, not a big deal really.

This topic is hashed over quite thoroughly in this thread link below, but if you get stuck with particulars, just ask away here.

http://www.cnczone.com/showthread.php?s=&threadid=706

[John F]

HU,

Thanks I think. I didn't try the bandit postprocessor is it what you used or have you extesivly altered it?

I will look at that thread and see if it helps

could you send me a copy of your post processor so that I can look at it and maybe alter it and use it. We won't have any problems with old files since I haven't produced any we would reuse yet. Another problem I ran into was two G codes on one line but that was easily fixed.

[HuFlungDung]

I have attached my file for anyone (with Onecnc XP series) to look at.

I do not believe that the default Bandit2 or Bandit4 posts are set up similarly to mine. In fact, let me know if you have a problem even opening my post in case of file incompatability. I am running a beta test version right now, is all, and I cannot guarantee backwards compatability.

For sure, the placement of the "/" for rapids will not work with your current version, but you can edit those out as I am sure they would not be useful to you. Be warned that Bandit post processors are quite far off the mainstream, so I wouldn't recommend that you use it, other than to run it to see how it works.

[John F]

HU,

Thanks I will.

In the meantime I found my problem. in the wizard I had Automatic/custom selected, changing that to machine cycles fixed my problem. so I now will most likely go back to trying the other post processors that are similar to our controls.

:cheers:

[HuFlungDung]

Ah yes, that would give you quite different results

[John F]

How do you add a Pic under your name in the side bar?

[cncadmin]

Originally posted by John F
How do you add a Pic under your name in the side bar?

http://www.cnczone.com/misc.php?s=&a...&page=1#avatar

[John F]

HU

Yes the post is different but not too different from mine except the G codes not being there.

All post processors that I tried had several problems with what our machines could read.

1) no double G or M codes on the same line

2) G83 is set up like this for example

G83 X Y Z B I K F

Where
X Dwell
Y Clearence
Z Final Depth
B Initial Clearence
I reduction in peck
K Peck

3) no G86 for boring bar boring

[wms]

Originally posted by John F
HU

Yes the post is different but not too different from mine except the G codes not being there.

All post processors that I tried had several problems with what our machines could read.

1) no double G or M codes on the same line

2) G83 is set up like this for example

G83 X Y Z B I K F

Where
X Dwell
Y Clearence
Z Final Depth
B Initial Clearence
I reduction in peck
K Peck

3) no G86 for boring bar boring

John,
Here is a modified Siemans post. I've only changed the G83 drill cycle. See if we are close to what you want.

Let me know and then we can work on this and the boring cycle.

[John F]

HU,
Thanks I'll take a look at it later today (I've got Cimatron programming to do)

I believe I have gott most of the bugs worked out. And I've already created a G86. It just finally clicked and I think I understand 90% of what I am doing for configuring the post processor.

[John F]

WMS,


My appologies. I thanked HU for the last post file.


Thank you the post is very close to what I have figured out.
Yesterday evening the configure of post just clicked and I think I've got about 90% done now. Just have to fix a few quirks as they come up with new situations.

[wms]

John,
No problem.
Glad it is working out for you. As always just takes a little time.

Happy Configing.