CamBam
News:
 
*
Welcome, Guest. Please login or register.
Did you miss your activation email?
June 18, 2018, 00:59:48 am


Login with username, password and session length


Pages: [1] 2
  Print  
Author Topic: 4th Axis Problems  (Read 386 times)
needleworks
CNC Ewok
*
Offline Offline

Posts: 19


View Profile
« on: June 12, 2018, 14:09:50 pm »

Once again I am needing some advice guys. I have successfully machined faces (skulls) on small pistons for a couple of years now, but at the weekend after a few months from doing my last one, I done the usual > load a dxf into cambam, using either cambam's own plugin, or cnc wrapper I then convert Y axis to the A axis > load the converted file into Mach3, only now, all I get is a series of random circles.

My Mach3 settings have not changed, apart from downgrading to version 62 (after the recent windows update) but everything is still set up the same.

No matter what I try, I cannot get a readable code. After doing at least 30 of these pistons over the last couple of years, it has me completely stumped!!

Does anyone have any experience of this happening since upgrading to Windows 10 Version 1803 ? Would anyone who has already upgraded to Version 1803 be prepared to draw a simple shape and try the conversion to wrap it and see how it turns out ?

Thanks in advance guys Smiley
Logged
jim1108
Droid
**
Offline Offline

Posts: 50


View Profile
« Reply #1 on: June 12, 2018, 14:52:23 pm »

I just did some skulls with rotary wrap on some 3 inch S.S. tubing the other day.
Windows version 1803, CB ver. 1.0(it has rotary integrated in it).
I uploaded a Version 1.0 fanuc rotary post in the post processor forum that works well, but with 1.0 only.
It should work with Mach 3 (dry run first) and Haas controls.
Upload your cb file so we can take a look at it.
Logged
Bob La Londe
CNC Jedi
*****
Offline Offline

Posts: 3249


^ 8.5 pounds on my own hand poured bait.


View Profile WWW
« Reply #2 on: June 12, 2018, 16:00:33 pm »

There is a patch for Mach3 so it continues to run under W10. 

https://www.cnczone.com/forums/cnc-router-parts/360698-cnc.html

Crop circles are just about always a result of arc settings, but I seem to recall that with wrapper you needed convert your curves to lines for it to work cleanly. 
Logged

Getting started on CNC?  In or passing through my area?
If I have the time I'll be glad to show you a little in my shop. 

Some Stuff I Make with CamBam
http://www.CNCMOLDS.com
needleworks
CNC Ewok
*
Offline Offline

Posts: 19


View Profile
« Reply #3 on: June 14, 2018, 09:18:32 am »

Yeah, I have already downgraded my Mach3 from Version 66, down to Version 62 and applied the patch, still no difference. I am gonna try and upload the CB file and also the code before and after converting to rotary using cnc wrapper.

* Skull.cb (6.99 KB - downloaded 6 times.)
* eyes_nose.nc (11.13 KB - downloaded 3 times.)
* eyes_nose - WRAPPED.nc (11.15 KB - downloaded 4 times.)
Logged
Bubba
CNC Jedi
*****
Offline Offline

Posts: 2429



View Profile
« Reply #4 on: June 14, 2018, 11:22:14 am »

I have already downgraded my Mach3 from Version 66, down to Version 62
********************
Version 62 is recommended version because v66 is buggy..
Logged

My 2¢
kvom
CNC Jedi
*****
Offline Offline

Posts: 1467


View Profile
« Reply #5 on: June 14, 2018, 15:39:01 pm »

I converted my mill from Mach3 to PathPilot and have never been happier.   Grin
Logged
dh42
Administrator
CNC Jedi
*****
Offline Offline

Posts: 4991



View Profile WWW
« Reply #6 on: June 14, 2018, 15:56:59 pm »

Hello,

I just have a look on your Gcode and I can see that the file contain G2 (arcs)

The Gcode must not contain arcs (G2, G3), because arcs can't be wrapped ; the code must contain only G0 and G1 (strait moves)

To solve this pb, change the Options - Arc Output property of your post processor to convert to lines, so arcs will be automatically converted to a series of small lines.

++
David

Note: this is true for all wrapping methods (CNC Wrapper, Wrapper plugin)

If you're using the built-in wrapper method of CB 1.0 post pro, it is not necessary to set this property to convert to line, If Rotary Wrap is set to True, the post processor will convert all toolpaths to lines only, then wrap all the toolpaths selected around the rotary axis. (it use stock surface of the MOP as radius to wrap)
« Last Edit: June 14, 2018, 16:07:56 pm by dh42 » Logged
needleworks
CNC Ewok
*
Offline Offline

Posts: 19


View Profile
« Reply #7 on: June 15, 2018, 10:05:06 am »

Thanks David, I have tried modifying the pp to convert arcs to lines but it's still not working !
Can you tell me how to access the built in wrap function in cambam v1.0 ? I haven't seen that so far.
« Last Edit: June 15, 2018, 10:08:44 am by needleworks » Logged
lloydsp
CNC Jedi
*****
Online Online

Posts: 7530



View Profile
« Reply #8 on: June 15, 2018, 11:55:06 am »

Let's see your post-processor!  After you changed the arc-output property, did you re-load your post processor?

Did you look at the g-code to see if it still contains G2 or G3?

A little more about "it still doesn't work" would be helpful.  What are the results, error messages, etc?

Lloyd
Logged

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

Posts: 19


View Profile
« Reply #9 on: June 15, 2018, 14:51:56 pm »

Sorry, I should maybe have been more specific regards not working, I have indeed re-loaded the pp's.
There are no G2 or G3 moves in the code but when I load it into Mach3 it either comes out as a load of random circles or just a straight line. I have tried dry cutting these and they are nowhere near what they are supposed to be.
The annoying thing for me is that I have cut dozens of these, but now all of a sudden I can't get anything to work!

Here is my Post and also the before and after wrapping code conversions.

* Mach3-CncWrapper.cbpp (0.92 KB - downloaded 0 times.)
* Skull pockets.nc (24.66 KB - downloaded 1 times.)
* Skull pockets - WRAPPED.nc (24.14 KB - downloaded 1 times.)
Logged
dh42
Administrator
CNC Jedi
*****
Offline Offline

Posts: 4991



View Profile WWW
« Reply #10 on: June 15, 2018, 15:26:00 pm »

Hello

I can get wrapped toolpaths on Mach3 (pic1) with you file, but an error remain with Z position ; in the Gcode header I can see (JOB DIAMETER = 49.66), but in the code, all Z values are close to 0 or < to 0 (Z=0 is the rotation center of the 4th axis), and the max Z height is +1 (so IN the stock) ... for a part with this diameter, the Z value for an engraving job on a cylinder must be close to the radius value and the Z clearance must be > to the radius. I guess that you have a problem in your MOP settings or in CNC wrapper settings. (I don't use CNC Wrapper so I don't remember how it works, I use the Wrapper plugin)

my Mach3 settings are:

In config/toolpath:
  Axis of rotation > X axis
  A Rotation enabled > checked

In General config, rotational section > all three settings unchecked

I would be fine if you can also share the .cb file (the one in the previous message contain only a drawing, the pocket MOPs are missing)

++
David

PS: to use the internal wrapping system of the V1.0, you need to do some change in the PP, but currently the explanations are only in French ; I'll will translate them when time permit.  Wink


* pic1.jpg (39.27 KB, 643x500 - viewed 3 times.)
« Last Edit: June 15, 2018, 15:39:55 pm by dh42 » Logged
dh42
Administrator
CNC Jedi
*****
Offline Offline

Posts: 4991



View Profile WWW
« Reply #11 on: June 15, 2018, 15:37:30 pm »

Re

I retrieve an old video here

https://www.youtube.com/edit?o=U&video_id=zH8miXGSdus

I guess that your problem is with stock surface, clearance plane and target depth values in the MOPs.

To wrap the drawing around a cylinder of 49.66mm Ø, you must set:

Stock surface = radius (24.83)
Clearance plane = above the radius .. i.e. = 30
Target depth = radius - pocket depth > so for a pocket = 2mm deep, 24.83-2 = 22.83

++
David
Logged
needleworks
CNC Ewok
*
Offline Offline

Posts: 19


View Profile
« Reply #12 on: June 15, 2018, 16:27:33 pm »

Thanks again David, I don't understand how to share the cambam file with the MOP's on it Cry

I have however tried doing what you suggested regarding the heights and I'm still having issues, I have included a jpeg of the toolpath I am getting.


* IMG_2286 copy.jpg (242.95 KB, 1000x750 - viewed 9 times.)
Logged
dh42
Administrator
CNC Jedi
*****
Offline Offline

Posts: 4991



View Profile WWW
« Reply #13 on: June 15, 2018, 16:42:41 pm »

Quote
Thanks again David, I don't understand how to share the cambam file with the MOP's on it

Just save your .cb file you have used to do your Gcode, and attach it to the message, it's the same as you do on reply #3, but in the file on reply #3 no machining operation is defined, it contain only the polylines.

I get the same as your picture, if "A rotation" is disabled in Config/toolpath

++
David
Logged
needleworks
CNC Ewok
*
Offline Offline

Posts: 19


View Profile
« Reply #14 on: June 16, 2018, 12:32:20 pm »

As requested, hopefully this is the proper cb file ?

* Skull Sockets.cb (9.4 KB - downloaded 4 times.)
Logged
Pages: [1] 2
  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 0.387 seconds with 20 queries.

Copyright © 2018 HexRay Ltd. | Sitemap