CamBam
News:
 
*
Welcome, Guest. Please login or register.
Did you miss your activation email?
September 19, 2019, 13:26:40 pm


Login with username, password and session length


Pages: [1]
  Print  
Author Topic: Post-processor for NCStudio 5.5.60 ?  (Read 256 times)
bartwaw
CNC Ewok
*
Offline Offline

Posts: 10


View Profile
« on: September 13, 2019, 11:40:48 am »

Hi,
i'm trying to run it on my friends machine that has NCstudio (5.5.60) controller.
For now without success.
Maybe someone is working on such controller ?

Logged
lloydsp
CNC Jedi
*****
Offline Offline

Posts: 7987



View Profile
« Reply #1 on: September 13, 2019, 12:08:17 pm »

Bart,
There are a lot of good post-processor writers here.  If you could upload or point us to the programming info for it, I'm sure you'd get some help.

Lloyd
Logged

"Pyro for Fun and Profit for More Than Fifty Years"
bartwaw
CNC Ewok
*
Offline Offline

Posts: 10


View Profile
« Reply #2 on: September 13, 2019, 15:23:58 pm »

Found problem with post-processor.

Changed G81 in settings from:
{$g81} {$_x} {$_y} {$_z} {$r} {$_f}

to
 
{$g81} {$x} {$y} {$_z} {$r} {$_f}

I't looks that NCstudio need all coordinates. As I suppose, "_" instructs cambam to not generate coordinate when not changed.
Am I right ?

Now must find how to change post-processor that NCStudio will accept feed rates.
For now it cuts at full speed, feedrates must be changed manually.



« Last Edit: September 13, 2019, 15:29:52 pm by bartwaw » Logged
Dragonfly
CNC Jedi
*****
Online Online

Posts: 2154



View Profile
« Reply #3 on: September 13, 2019, 15:41:17 pm »

Does NCStudio not accept G0 and G1 commands? I've seen it only on one large flatbed router used for cutting and grooving  sheets of Al-Plastic-Al sandwich sheets used for building decoration. It mimics the way Canadian AXYZ routers work for the same purpose and they have some "slang" of G-code of their own. Bu still, they do accept G0 and G1.
Logged
Dragonfly
CNC Jedi
*****
Online Online

Posts: 2154



View Profile
« Reply #4 on: September 13, 2019, 15:44:06 pm »

Here you can read and save NCStudio programming manual. No matter rhe version they should have similar functionality.
http://doc.weihong.com.cn:8880/NcStudio%20Programming%20Manual-R6.1.pdf
Logged
lloydsp
CNC Jedi
*****
Offline Offline

Posts: 7987



View Profile
« Reply #5 on: September 13, 2019, 16:45:24 pm »

I haven't read the whole manual, but went over the commands it accepts.  It looks pretty 'generic'.  It has some Weihong-specific commands, but the basic set is the same as most generic NC machines.

Almost any very-simple post-processor should work.  What are you trying that gives you 'no luck'?

Lloyd
Logged

"Pyro for Fun and Profit for More Than Fifty Years"
bartwaw
CNC Ewok
*
Offline Offline

Posts: 10


View Profile
« Reply #6 on: September 13, 2019, 17:05:07 pm »

I'm already analyzing that manual.

Previously G81, G82 and G83 were generated by cambam in some places without X or Y.
NCStudio as i suppose need X and Y in G81.

I've changed as i said to:
{$g81} {$x} {$y} {$_z} {$r} {$_f}


Logged
dh42
Administrator
CNC Jedi
*****
Offline Offline

Posts: 5550



View Profile WWW
« Reply #7 on: September 14, 2019, 02:13:26 am »

Hello

Quote
Almost any very-simple post-processor should work.  What are you trying that gives you 'no luck'?

Yes, the "default" one seems to be the closest (better that mach3 pp)

It seems also that G61/64 are missing in NCstudio GCode. (exact stop/constant velocity)

remove the {$velocitymode} macro in the post processor header to remove the output of G61/64

if you find a {$arccentermode} macro in the PP you're using, remove it too.

++
David
« Last Edit: September 14, 2019, 02:18:00 am by dh42 » Logged
bartwaw
CNC Ewok
*
Offline Offline

Posts: 10


View Profile
« Reply #8 on: September 14, 2019, 06:39:43 am »

Hello,
removed  {$velocitymode}

This is how it looks. Will try today this PP.


Code:
  <PostFile>{$comment}NCStudio_post {$endcomment}
{$header}
{$mops}
{$footer}
</PostFile>
  <Header>{$comment} {$cbfile.name} {$date} {$endcomment}
{$tooltable}
{$cbfile.header}
{$units} {$distancemode} {$cuttercomp(off)}
{$toolchange(first)}
{$clearance}


</Header>
  <Footer>{$clearance}
{$spindle(off)}
{$endrewind}
{$cbfile.footer}
</Footer>
  <ToolTableItem>{$comment} Frez-mm-: {$tool.diameter} {$endcomment}
{$comment} T{$tool.index}  {$endcomment}</ToolTableItem>
  <ToolChange>{$clearance}
{$comment} {$tool.diameter} {$endcomment}
</ToolChange>
  <MOP>{$comment} {$mop.name} {$endcomment}
{$workplane}
{$mop.header}
{$spindle} {$s}
{$blocks}
{$mop.footer}
</MOP>
  <EndRewind>G91
G0 Z10
G0
G4 P2
G0 X0 Y0
M30</EndRewind>
  <Rapid>{$g0} {$_x} {$_y} {$_z} {$_f} {$_a} {$_b} {$_c}</Rapid>
  <FeedMove>{$g1} {$_x} {$_y} {$_z} {$_f} {$_a} {$_b} {$_c}</FeedMove>
  <ArcCW>{$g2} {$_x} {$_y} {$_z} {$i} {$j} {$k} {$_f}</ArcCW>
  <ArcCCW>{$g3} {$_x} {$_y} {$_z} {$i} {$j} {$k} {$_f}</ArcCCW>
  <Drill>{$g81} {$x} {$y} {$_z} {$r} {$_f}</Drill>
  <DrillDwell>{$g82} {$x} {$y} {$z} {$r} {$p} {$_f}</DrillDwell>
  <DrillPeck>{$g83} {$x} {$y} {$z} {$r} {$q} {$_f}</DrillPeck>
  <NumberFormat>0.###</NumberFormat>
  <MaximumArcRadius>10000</MaximumArcRadius>
  <SuppressParserErrors>true</SuppressParserErrors>
  <AddLineNumbers>true</AddLineNumbers>
</PostProcessor>
Logged
Pages: [1]
  Print  
 
Jump to:  

Powered by MySQL Powered by PHP Powered by SMF 1.1.21 | SMF © 2015, Simple Machines

Valid XHTML 1.0! Valid CSS! Dilber MC Theme by HarzeM
Page created in 0.128 seconds with 19 queries.

Copyright © 2018 HexRay Ltd. | Sitemap