CamBam
News:
 
*
Welcome, Guest. Please login or register.
Did you miss your activation email?
November 20, 2017, 05:44:32 am


Login with username, password and session length


Pages: [1] 2 3 ... 14
  Print  
Author Topic: customised post processor  (Read 23456 times)
michel
Storm Trooper
***
Offline Offline

Posts: 219



View Profile WWW
« on: December 30, 2015, 09:55:02 am »

Hi ,

I just downloaded cambam and it looks very similar to a program I currently use ( Heekscnc ) . Until today It was ok as a program but I am looking to have a more performing software and I think that cambam is one of these. My problem is that I cannot program my own  postprocessor. Just not enough knowledge I guess Grin.

What I do have is the postprocessor made for my machine in heekscnc . Is there someone that can help me to setup this postprocessor on cambam so that I can start testing on my machine ? Maybe the postprocessor from heekscnc can be used ??

Another important question which i did not found in the documentation is . As I am a stairbuilder I have several parts to be produced ( milling) . With heekscad I had to make a dxf file of each idividual part on the exact 0,0,0 co÷rdinates of the drawing sheet ( autocad). This because heekscnc only use that point as a zero reference. Does cambam give me the possibility to import a sheet with 10 different parts on that I can post process one by one and select the same machine zero point ( floating point ) for each of these parts ? I would put on each part a point representing the zero point . When I postprocess I would like to have the possibility to select that specific point to be the zero point for that specific part . I hope it was clear to understand  Huh


regards
Michel
Logged
lloydsp
CNC Jedi
*****
Offline Offline

Posts: 7155



View Profile
« Reply #1 on: December 30, 2015, 12:10:06 pm »

Michel,
It would be worthwhile for us to look at your post processor, but it's unlikely that yours would bear any resemblance to a CamBam post processor.  Please do post yours, but if you have a link to the manual for your cnc machine, that will be of the most use for us to help.

For your 'multiple parts', it is entirely possible to have multiple parts with the same origins in what CamBam calls 'layers'.  It's also possible to re-reference parts so that they may be machined somewhere other that at the origin.

When we see an example of what you wish to accomplish, I'm sure we can instruct you on how to accomplish it in CamBam.

LLoyd
Logged

"Pyro for Fun and Profit for More Than Fifty Years"
michel
Storm Trooper
***
Offline Offline

Posts: 219



View Profile WWW
« Reply #2 on: December 30, 2015, 12:47:50 pm »

Hi ,


ok thanks I hope it will work . I attached here 3 files . iso.py which is the min file of the postprocessor used for my machine . I think it was similar to the linux processor .  the second one is reichenbacher.py . This is written to create a certain output needed for my machine . It works with that . THe third one is just a test  code . With this output the machine is running correctly . Machine is a 3 axis reichenbacher ranc 230 .

does cambam also runs on open shapes ?  With stairs a stringer can be long and i have to mill it in 2 steps so this creats open ends.


regards
Michel 

* ReichenbacherRanc323py.txt (2.61 KB - downloaded 77 times.)
* test.txt (2.62 KB - downloaded 92 times.)
* isopy.txt (55.33 KB - downloaded 70 times.)
Logged
lloydsp
CNC Jedi
*****
Offline Offline

Posts: 7155



View Profile
« Reply #3 on: December 30, 2015, 13:17:58 pm »

"...does cambam also runs on open shapes ?  With stairs a stringer can be long and i have to mill it in 2 steps so this creats open ends."

------------
Yes, CB can do 'open profiles'.  That's quite a machine you have there!

I don't see much in that post that is unusual, but I either do not know or have forgotten what the "D#" accompanying a tool-change is for.  It seems like it always matches the tool number, so it would be easy to do in CB.  I'm guessing it references a tool index in the machine's tool table, but don't know that to be the case.

I see that your post only permits up to three actual tools, plus tool #0.  You will be able to refer to many more tool numbers in CB, if your machine can recognize higher numbers than T3.

I'll fiddle with a sample post today.  If there's anyone else out there familiar with the Ranc 230, please offer your opinions!

Michel, if you have the g-code programming information for the machine, it will be more helpful than anything else you can give us.

Lloyd
Logged

"Pyro for Fun and Profit for More Than Fifty Years"
kvom
CNC Jedi
*****
Offline Offline

Posts: 1388


View Profile
« Reply #4 on: December 30, 2015, 13:18:35 pm »

The generated code in the 2nd file looks reasonably generic.  Would the move codes work with spaces between the words?  E.g., G1 X1 vs. G1X1

As for the stringers, yes CB can mill profiles along open polylines.  You'd split the stringer into two separate polylines, mill the first, move the stock, and then mill the second.  Pretty much what you do now.

LLoyd posted same time as I.  The D code typically refers to the tool diameter in a tool table, and is needed only if the code is using offsets.  CB does not use offsets, but your code doesn't have the normal G41 or G42 for setting this.
« Last Edit: December 30, 2015, 13:22:30 pm by kvom » Logged
kvom
CNC Jedi
*****
Offline Offline

Posts: 1388


View Profile
« Reply #5 on: December 30, 2015, 13:25:59 pm »

Here's a video of this machine

https://www.youtube.com/watch?v=1QdeZhcxYO4
Logged
michel
Storm Trooper
***
Offline Offline

Posts: 219



View Profile WWW
« Reply #6 on: December 30, 2015, 14:04:28 pm »

Hi ,

No this is not the machine . I attached the picture of a similar one but my table is 230 cm long

I have a programming guide of the machine but the file is too large to attache but you can find it if you google

sinumerik 3m manual. In the reults shoiuld appear a pdf called sinumerik system 3 . If you open it it is called  sinumerik System 3  basic version 4C

or in case i Can get an email i will forward it from my email .

D02 per example stands for the second tool T2 is the second spindle .  this is always used in combination with G59 x220 which is the location of the spindle related to the machine 0 point . M82 I can not explain but it is also needed for the second spindle and S155 represent the spindle speed . CB should not output any spindle speed.


About the offset when I use heekscnc that program is doing the offset . This is the reason why it is not visible as g41 and g42


regards
Michel


* ranc230.png (513.24 KB, 779x537 - viewed 110 times.)

* ranc230.png (513.24 KB, 779x537 - viewed 104 times.)
Logged
michel
Storm Trooper
***
Offline Offline

Posts: 219



View Profile WWW
« Reply #7 on: December 30, 2015, 14:24:22 pm »

Hi


About the G41  case . There was a person making my gcodes before I switched to heekscad and this code was in my opinion much better then the heekscnc one . I attached a example and there you can see the use of G41. I also attached a worksheet . This is what i would load into cb to generate separate gcodes for each individual part starting from their own positioned point and these would all have the same origin ( machine  0 point ).



hope this helps .
Already thanks a lot for the assistance I get on this

* worksheet.pdf (148.01 KB - downloaded 63 times.)
* 107.NC (3.61 KB - downloaded 58 times.)
Logged
lloydsp
CNC Jedi
*****
Offline Offline

Posts: 7155



View Profile
« Reply #8 on: December 30, 2015, 14:50:54 pm »

PM sent, Michel.

Lloyd
Logged

"Pyro for Fun and Profit for More Than Fifty Years"
lloydsp
CNC Jedi
*****
Offline Offline

Posts: 7155



View Profile
« Reply #9 on: December 30, 2015, 16:14:46 pm »

Michel sent me the pdf for the manual, and except for setup stanzas, I believe it's a pretty generic machine.

Like a lot of older machines, the control seems to support LOTS of built-in compute-intensive cycles that were designed for the older 'hand programmed' methods.  But it supports all the basic stuff, too.

Attached below, for comments, split in two parts (and two replies) for size.

Lloyd

* Programming_Guide_3M-pt1.pdf (2755.44 KB - downloaded 97 times.)
Logged

"Pyro for Fun and Profit for More Than Fifty Years"
lloydsp
CNC Jedi
*****
Offline Offline

Posts: 7155



View Profile
« Reply #10 on: December 30, 2015, 16:18:10 pm »

part2
L

* Programming_Guide_3M-pt2.pdf (2830.99 KB - downloaded 71 times.)
Logged

"Pyro for Fun and Profit for More Than Fifty Years"
lloydsp
CNC Jedi
*****
Offline Offline

Posts: 7155



View Profile
« Reply #11 on: December 30, 2015, 19:41:23 pm »

Ok... there are a couple of things, one minor, one major.

The major one is that the machine has very limited memory, so in addition to a post-processor, we should also add a post-build processor that checks the file-size, and reports to the user whether or not it's greater than the memory limit.  CB can't control it, but at least we can 'sense' it and report it.

The minor one is 'mentally bothersome', but likely not an issue.  The machine uses cutter-radius compensation which must be based upon the direction of cut (climb or conventional).  On a metal-working machine cutting to within a 'tenth', I would say this is pretty important.

But I cannot see the utility of it on a wood-cutting machine, unless there is some SERIOUS play in the positioning mechanisms.  To that end, I asked Michel about the positioning devices, and he indicates they are ball screws, and in good condition.

So based upon that, I think adding the compensation would not really be necessary -- and some of his code examples do not use it.   Further, I don't know of any way CB can report to the post that the cut is in climb or conventional, so there's no real 'programmatic' way to add that feature.

Ideas? Comments?

Lloyd
Logged

"Pyro for Fun and Profit for More Than Fifty Years"
michel
Storm Trooper
***
Offline Offline

Posts: 219



View Profile WWW
« Reply #12 on: December 30, 2015, 19:55:32 pm »

Hi Lloyd,

i do not have any check on file size in the programs I used before . I guess you should not consider that . My max file sizes are around 8k and I see that before I even attend to upload the files.

If i tell you that profiling (outside cutting ) is always clockwise and that pocket ( inside cutting) is always counterclokwise is that something that can be used ?

I attached the screen i get on heeks when i do profile operations and there you see the possibility on cut mode and tool on side . With this program there is not g41 code in the gcode



* profileoperation.jpg (70.62 KB, 571x592 - viewed 111 times.)

* Profile Operation2.jpg (70.95 KB, 571x599 - viewed 105 times.)
Logged
lloydsp
CNC Jedi
*****
Offline Offline

Posts: 7155



View Profile
« Reply #13 on: December 30, 2015, 20:10:13 pm »

If i tell you that profiling (outside cutting ) is always clockwise and that pocket ( inside cutting) is always counterclokwise is that something that can be used ?
------------
Indeed, that is useful.  It says you always cut in "climb", and if so, just automatically inserting the compensation code for climb should at least marginally improve the cut accuracy.

However, you must be careful to set up a regimen of always specifying 'climb' in the cut direction of any cut.  CB defaults to 'conventional' unless you change the template.  (That, because it's the direction least-likely to be affected by lash in the positioning mechanism... a hold-over from old Acme-thread feeds.)

LLoyd
« Last Edit: December 30, 2015, 20:13:33 pm by lloydsp » Logged

"Pyro for Fun and Profit for More Than Fifty Years"
kvom
CNC Jedi
*****
Offline Offline

Posts: 1388


View Profile
« Reply #14 on: December 30, 2015, 21:20:31 pm »

If it's the machine that does compensation rather than his current CAM, then the first question is whether it's optional.  If not, then he can use CB without it.

If compensation is always used, then there are two options.  One, set the tool diameter to either zero or a very small number in the tool table and use CB normally. 

Second, keep the tool diameter in the machine tool table and specify a tool diameter very small in CB. 
Logged
Pages: [1] 2 3 ... 14
  Print  
 
Jump to:  

Powered by MySQL Powered by PHP Powered by SMF 1.1.19 | SMF © 2013, Simple Machines

Valid XHTML 1.0! Valid CSS! Dilber MC Theme by HarzeM
Page created in 0.142 seconds with 18 queries.

Copyright ┬ę 2008 HexRay Ltd. | Sitemap