Denford Software & Machines

Denford Software & Machines

 
 

Denford Software & Machines

Welcome to the Denford CAD CAM CNC forum


Hint - Try the google search at the bottom of the page
It is currently Thu 30 Mar , 2017 21:18 pm

All times are UTC [ DST ]




Post new topic Reply to topic  [ 13 posts ] 
Author Message
 Post subject: Circles/arcs
PostPosted: Tue 03 Mar , 2009 14:38 pm 
Offline

Joined: Fri 14 Mar , 2008 14:29 pm
Posts: 14
Location: East Yorkshire
Hi

when we draw a circle and export to machine it cuts anti clockwise...is there a way we can set the default to so it will run clockwise each time....when we cut perspex it cuts a much cleaner circle running clockwise because of the cutting edge on the tooling

thanks

Phill


Top
 Profile  
 
 Post subject:
PostPosted: Tue 03 Mar , 2009 17:25 pm 
Offline
Site Admin
User avatar

Joined: Fri 10 Feb , 2006 12:40 pm
Posts: 3571
Location: Sunny Brighouse Hardware/Software: Go to User Control Panel > Profile
Enter as much information about your CNC hardware and software as you can - it makes it easier for everyone to know what you're talking about then.
Are you using the older version of Techsoft ? The one that uses the Denford/Techsoft extension ?
If so, then there could be a way to alter the Denford extension to look for circles and output G02 instead of G03 (or vice versa)...
Can you create an example output , and supply the file GENERIC.GNC which will be located here:
C:\Denford\Data


Top
 Profile  
 
 Post subject:
PostPosted: Fri 06 Mar , 2009 12:56 pm 
Offline

Joined: Fri 14 Mar , 2008 14:29 pm
Posts: 14
Location: East Yorkshire
Hi

we are using V2...and then export as a design tools transfer file so we can plot to a microuter from V1


Top
 Profile  
 
 Post subject:
PostPosted: Fri 06 Mar , 2009 13:06 pm 
Offline
Site Admin
User avatar

Joined: Fri 10 Feb , 2006 12:40 pm
Posts: 3571
Location: Sunny Brighouse Hardware/Software: Go to User Control Panel > Profile
Enter as much information about your CNC hardware and software as you can - it makes it easier for everyone to know what you're talking about then.
In that case, then this may work:
I looked at the post config file, and it seems as though arc angles greater than 0 output G03 and any others are G02.
I'm not sure what specifies a circle, but if its an angle of 0, then G02 will always be specified.
Locate this file
C:\Denford\Libs\Fanucm.slb
Make a copy of it !

Then have a look for this bit of code:

Code:
* Circular traverse
proc circ_trav
....
    if angle > 0
      gcode = 3
    else
      gcode = 2
    endif
..
return circ_trav


Possibly changing this little bit will fix it if circles are specified with a 0 degree angle (and not 360)

Code:
    if angle >= 0
      gcode = 3
    else
      gcode = 2
    endif


I'd need to see a .GNC file with circles in to be sure what will fix it though.


Top
 Profile  
 
 Post subject:
PostPosted: Fri 06 Mar , 2009 13:14 pm 
Offline
Site Admin
User avatar

Joined: Fri 10 Feb , 2006 12:40 pm
Posts: 3571
Location: Sunny Brighouse Hardware/Software: Go to User Control Panel > Profile
Enter as much information about your CNC hardware and software as you can - it makes it easier for everyone to know what you're talking about then.
sorry had to edit the last post a few times as the forum was loosing parts of the message. ... you might want to refresh it and read it again..


Top
 Profile  
 
 Post subject:
PostPosted: Tue 17 Mar , 2009 11:47 am 
Offline

Joined: Fri 14 Mar , 2008 14:29 pm
Posts: 14
Location: East Yorkshire
is this what you need?

and many thanks for your help on this subject

phill



string machine_type (4)="MILL"
repeat
metric=TRUE
real x_datum=0
real y_datum=0
real z_datum=0
real x_dimension=80
real y_dimension=80
real z_dimension=13.2
PROJECT="TechSoft Design Tools - Untitled1"
DATE="17.03.2009"
PROGID=99
PROLOGUE
no_of_tools=1
tool=1
tool_diam=0.3
tool_length=0
DEFINE_TOOL
tools_defined
tool=1
tool_diam=0.3
tool_length=0
CHANGE_TOOL
spindle=15000
CHANGE_SPINDLE
x=9.43624
y=7.73154
FAST_TRAV
z=2
FAST_TRAV
z=-0.800001
feed=300
LINEAR_TRAV
x=70.1208
y=7.73154
feed=1200
LINEAR_TRAV
cx=70.1208
cy=9.73154
angle=90
feed=1200
CIRC_TRAV
x=72.1208
y=70.1208
feed=1200
LINEAR_TRAV
cx=70.1208
cy=70.1208
angle=90
feed=1200
CIRC_TRAV
x=9.43624
y=72.1208
feed=1200
LINEAR_TRAV
cx=9.43624
cy=70.1208
angle=90
feed=1200
CIRC_TRAV
x=7.43624
y=9.73154
feed=1200
LINEAR_TRAV
cx=9.43624
cy=9.73154
angle=90
feed=1200
CIRC_TRAV
z=-1.6
feed=300
LINEAR_TRAV
x=70.1208
y=7.73154
feed=1200
LINEAR_TRAV
cx=70.1208
cy=9.73154
angle=90
feed=1200
CIRC_TRAV
x=72.1208
y=70.1208
feed=1200
LINEAR_TRAV
cx=70.1208
cy=70.1208
angle=90
feed=1200
CIRC_TRAV
x=9.43624
y=72.1208
feed=1200
LINEAR_TRAV
cx=9.43624
cy=70.1208
angle=90
feed=1200
CIRC_TRAV
x=7.43624
y=9.73154
feed=1200
LINEAR_TRAV
cx=9.43624
cy=9.73154
angle=90
feed=1200
CIRC_TRAV
z=-2.4
feed=300
LINEAR_TRAV
x=70.1208
y=7.73154
feed=1200
LINEAR_TRAV
cx=70.1208
cy=9.73154
angle=90
feed=1200
CIRC_TRAV
x=72.1208
y=70.1208
feed=1200
LINEAR_TRAV
cx=70.1208
cy=70.1208
angle=90
feed=1200
CIRC_TRAV
x=9.43624
y=72.1208
feed=1200
LINEAR_TRAV
cx=9.43624
cy=70.1208
angle=90
feed=1200
CIRC_TRAV
x=7.43624
y=9.73154
feed=1200
LINEAR_TRAV
cx=9.43624
cy=9.73154
angle=90
feed=1200
CIRC_TRAV
z=-3.2
feed=300
LINEAR_TRAV
x=70.1208
y=7.73154
feed=1200
LINEAR_TRAV
cx=70.1208
cy=9.73154
angle=90
feed=1200
CIRC_TRAV
x=72.1208
y=70.1208
feed=1200
LINEAR_TRAV
cx=70.1208
cy=70.1208
angle=90
feed=1200
CIRC_TRAV
x=9.43624
y=72.1208
feed=1200
LINEAR_TRAV
cx=9.43624
cy=70.1208
angle=90
feed=1200
CIRC_TRAV
x=7.43624
y=9.73154
feed=1200
LINEAR_TRAV
cx=9.43624
cy=9.73154
angle=90
feed=1200
CIRC_TRAV
z=2
FAST_TRAV
EPILOGUE
until last_pass


Top
 Profile  
 
 Post subject:
PostPosted: Tue 17 Mar , 2009 12:02 pm 
Offline
Site Admin
User avatar

Joined: Fri 10 Feb , 2006 12:40 pm
Posts: 3571
Location: Sunny Brighouse Hardware/Software: Go to User Control Panel > Profile
Enter as much information about your CNC hardware and software as you can - it makes it easier for everyone to know what you're talking about then.
Yep - thats the intermediate file which Techsoft creates, and the Denford post uses to create a CNC file.
It looks like Techsoft outputs a maximum of 90 degree arcs - it could well be splitting circles up so as not to go past any quadrants.

If this is the circle program, then only the Techsoft software could change the direction of circles.
Either with a setting, or possibly by drawing the circles differently ?
Might be worth putting the question to them...


Top
 Profile  
 
 Post subject: Re: Circles/arcs
PostPosted: Fri 13 Dec , 2013 10:15 am 
Offline

Joined: Mon 13 Aug , 2007 16:30 pm
Posts: 3
Hi,

We have a student who needs to machine a series of ovals on the Microrouter to construct a laminated box.
He has drawn them up in Techsoft 2D Design V2 version 2.10 and they appeared on screen as intended, and also cut out cleanly and to the correct size when he did a test run in thin card on the laser.

When we save as a dxf however and import into the Microrouter running VR Milling version 5.54.0.630 the drawing import cam page shows the design as whilst still being basically the correct shape, it is made up of a series of straight lines and not the smooth curves as originally drawn, and this new, incorrect tool path is confirmed in the next stages when the outer contour is selected, simulated and machined, this problem also occurs in another design involving a circle.

We have tried completely redrawing again with the same results, I am not sure what the “use arc command” is supposed to do when exporting from Techsoft 2D Design as a dxf, but it doesn’t seem to make any difference in this case whether it is used or not.

We tried taking a copy the same drawing and using the “Alter the size of the selected objects” command in the 2D Design toolbox, reduced its size to enable it to fit a piece of 160mm x 90mm HIPS, and then saved this as a dxf before importing it into the Triac and where it both simulated and machined perfectly.

I understand that if the drawing size is reduced, then any errors will also decrease proportionally, but the Triac version appears perfect, with no distinguishable defects at all.

Both the machines are networked and running windows 7 service pack 1, the only difference I can think of is the Triac is using a different version of VR Milling, as it currently has version 5.49.0.613 installed.

Is there a setting somewhere that controls the resolution when converting to G-code, does anyone know of any conflict with our version of 2D Design and the Microrouters version of VR Milling or are we missing an obvious point, because we have never had a problem like this before.


Top
 Profile  
 
 Post subject: Re: Circles/arcs
PostPosted: Fri 13 Dec , 2013 10:49 am 
Offline
CNC Guru
CNC Guru
User avatar

Joined: Tue 21 Feb , 2006 16:15 pm
Posts: 1190
Location: Denford UK
Hi,

I am not sure exactly what the problem you have is. When drawing in techsoft a lot of arcs are broken down into straight lines. I have tried exporting a circle and an elipse from Techsoft and importing into another package and the elipse comes through as a series of lines. This happens when exporting to corel or QuickCAM.

I am not sure why you have a problem with the arc being lines as it should still machine correctly if there are enough of them.

Can you post some screenshots showing the problem and a sample of DXF's. I think this is an issue with the Techsoft.

I am unsure as to why different versions of VR milling have a different result selecting a different machine will change nothing other than the material library selection.


Top
 Profile  
 
 Post subject: Re: Circles/arcs
PostPosted: Tue 17 Dec , 2013 12:49 pm 
Offline

Joined: Mon 13 Aug , 2007 16:30 pm
Posts: 3
Hi, thanks for the reply,

Here are the a couple of screen shots, dxf and a picture of the machined result, I tried to add the Techsoft 2D Design file but the forum won't allow the dtd extension.


Attachments:
Oval For Box.fnc [1.9 KiB]
Downloaded 407 times
Oval For Box.dxf [64.42 KiB]
Downloaded 443 times
Oval For Box Tool Path.docx [68.36 KiB]
Downloaded 424 times
Oval For Box 1.docx [65.85 KiB]
Downloaded 414 times
Oval For Box Machined.jpg
Oval For Box Machined.jpg [ 663.77 KiB | Viewed 14251 times ]
Top
 Profile  
 
 Post subject: Re: Circles/arcs
PostPosted: Tue 17 Dec , 2013 14:17 pm 
Offline
CNC Guru
CNC Guru
User avatar

Joined: Tue 21 Feb , 2006 16:15 pm
Posts: 1190
Location: Denford UK
Hi, I have tried opening the DXF in various packages and it apears to be OK. I had V 5.53 on my computer which worked fine. Have upgraded to 5.54 and have the same result as you do.

I will forward this to our software engineer and we will get it fixed and post a new version.

Short term either go back to your previous version or import the DXF into QuickCAM 2D and post process in that package.


Top
 Profile  
 
 Post subject: Re: Circles/arcs
PostPosted: Wed 18 Dec , 2013 13:30 pm 
Offline

Joined: Mon 13 Aug , 2007 16:30 pm
Posts: 3
Hi,

OK, thanks for the quick response; your help is very much appreciated,

Kev


Top
 Profile  
 
 Post subject: Re: Circles/arcs
PostPosted: Mon 06 Jan , 2014 15:40 pm 
Offline
Site Admin
User avatar

Joined: Fri 10 Feb , 2006 12:40 pm
Posts: 3571
Location: Sunny Brighouse Hardware/Software: Go to User Control Panel > Profile
Enter as much information about your CNC hardware and software as you can - it makes it easier for everyone to know what you're talking about then.
Hi. There is a new version of VR Milling available on the software download site at http://website.denford.ltd.uk/index.php ... -downloads. This version number is 5.55. The curves on loaded DXF files are smoothed off as expected. Can you please download and install this new version and see if that works better for you?


Top
 Profile  
 
Display posts from previous:  Sort by  
Post new topic Reply to topic  [ 13 posts ] 

All times are UTC [ DST ]


Who is online

Users browsing this forum: No registered users and 1 guest


You cannot post new topics in this forum
You cannot reply to topics in this forum
You cannot edit your posts in this forum
You cannot delete your posts in this forum
You cannot post attachments in this forum

Search for:
Jump to:  
Powered by phpBB © 2000, 2002, 2005, 2007 phpBB Group
Template made by DEVPPL
[ Time : 0.264s | 18 Queries | GZIP : Off ]
 
Loading