Arc converted to straight lines.

Submit any comments, issues or requests relating to the use of VR Milling Version 5 and 2

Moderators: Steve, Mr Magoo, Martin, bradders

MAX THE MILLER
CNC Apprentice
CNC Apprentice
Posts: 90
Joined: Tue 23 Aug , 2011 18:25 pm
Hardware/Software: Denford Triac PC. VR Milling 5.51.0.616

Arc converted to straight lines.

Post by MAX THE MILLER » Thu 11 Dec , 2014 17:19 pm

Using VR Milling version 5.59.0.666 with Triac PC.

I have attached .DWG and .DXF files for the same part, an oblong plate with one side being an arc of 203.2 mm (8 inch radius).

If I import either of these files into VR Milling, use it to create a .fnc file and then cut the part, the machine cuts four straight lines instead of the arc. These straight lines are clearly shown as G1 commands in the .fnc file which is also attached.

I thought perhaps there was a problem with the .DWG or .DXF file. I can't manually analyse the .DWG file as it's in binary format, however the .DXF file is an ASCII file with the arc clearly specified by centre point. radius and angle.

So it would appear that the problem is with VR Milling. Can this be fixed please.
Attachments
Coal Plate.fnc
(797 Bytes) Downloaded 425 times
Coal Plate.DXF
(58.52 KiB) Downloaded 585 times
Coal Plate.DWG
(77.29 KiB) Downloaded 421 times

TDIPower
CNC Guru
CNC Guru
Posts: 398
Joined: Tue 29 Apr , 2014 18:38 pm
Hardware/Software: Starturn 5 (sort of running, I will get this done!)
Lathe cam designer V1.11
Quickturn 2D Design
FANUC offline and online programs.
Microrouter Pro NS V5 (microstep)
VR2 and VR5
Boxford VMC260
Techsoft 2d Design tools V1 > V2
ProDesktop
Fusion 360
Deskproto

Re: Arc converted to straight lines.

Post by TDIPower » Thu 11 Dec , 2014 20:04 pm

Ive had an issue with the DXF to G code converter in VR5 for the micromill. I have found if I unselect/select the check box for something to do with Arc/Polyline (I think Im not at work so cant check) that it works. Basically I need to unselect what ever the default it to get the micromill to cut a radius.
If I don't do this the micromill has a hit and miss success rate on if it will cut it or hang the program.

I can see the difference in the G code, Im not sure what the code is telling it to do but can see the command is written in a different format and the 'tune' the steppers make carrying out the task sounds wrong in default.

Looking at your code for me the problem lies in the lines like this

G2 X-0.233Y18.944 I1.500J0.000

It's the ones with the I and J commands it doesn't like

MAX THE MILLER
CNC Apprentice
CNC Apprentice
Posts: 90
Joined: Tue 23 Aug , 2011 18:25 pm
Hardware/Software: Denford Triac PC. VR Milling 5.51.0.616

Re: Arc converted to straight lines.

Post by MAX THE MILLER » Thu 11 Dec , 2014 21:53 pm

Thanks for your reply.

Before posting I actually plotted the G Code on graph paper. Old fashioned, but it works. The G2 commands in the .fnc file are actually used to "ROLL" the 3mm diameter cutter round the corners of the part. Hence I=1.5, half the cutter diameter. Without these G2 commands the cutter would follow a longer path, losing contact with the outline of the part at the corners. This would result in longer machining times and more material being removed than necessary.

The "ARC" is actually cut by these commands:-

G1 X8.060Y20.247
X29.223Y22.020
X50.503Y21.589
X71.624Y18.951

The box you refer to is the "Convert Polylines to Arcs" box which is ticked by default. I'll try unticking it. As far as I'm concerned though I drew an arc, not a polyline. This box isn't documented in the help file and neither is the "Auto Join Entities" box.

I've actually cut many arcs using VR Milling 5 and have had no problems. However the arcs were of smaller radius and mostly multiples of 90 degrees.

I'm hoping Denford will fix this, but that isn't going to happen in the short term. If all else fails I'll edit the .fnc file to include an arc or resort to sawing and filing the part as I did before I had the Triac.

TDIPower
CNC Guru
CNC Guru
Posts: 398
Joined: Tue 29 Apr , 2014 18:38 pm
Hardware/Software: Starturn 5 (sort of running, I will get this done!)
Lathe cam designer V1.11
Quickturn 2D Design
FANUC offline and online programs.
Microrouter Pro NS V5 (microstep)
VR2 and VR5
Boxford VMC260
Techsoft 2d Design tools V1 > V2
ProDesktop
Fusion 360
Deskproto

Re: Arc converted to straight lines.

Post by TDIPower » Thu 11 Dec , 2014 23:24 pm

I don't really know G code, I want to learn more about it so I can program my Starturn rather than depend on the limited software I have.

I don't know the difference between polylines and arcs either! but by changing that option the micromill started to play the same 'tune' when machining that it did using VR2 and hasn't hung when machining since.

I did find that some of the setup information for the micromill was not correct in VR5 and it took an evening with 2 PCs going through all the setup info between VR2 and VR5 to resolve it.

Would be interesting to see if it does solve your issue though.

Pete

MAX THE MILLER
CNC Apprentice
CNC Apprentice
Posts: 90
Joined: Tue 23 Aug , 2011 18:25 pm
Hardware/Software: Denford Triac PC. VR Milling 5.51.0.616

Re: Arc converted to straight lines.

Post by MAX THE MILLER » Thu 11 Dec , 2014 23:42 pm

The help files provided with VR Milling 5 are very good when it comes to G Code. I find I can get on OK just knowing G0, G1, G2 and G3.

I suspect very few people actually write G Code directly these days, just as no one constructs a web page by writing directly in html. Instead they'll use some kind of CAM app to generate G Code from a CAD file.

I unticked the box and ran a simulation, which looks much better. However the .fnc file cuts the arc as a series of short straight lines (obviously the more and shorter the lines the better) and doesn't use G2 or G3 command for the arc which is what I'd expect.

I'll try actually machining a part at the weekend and report back.

MAX THE MILLER
CNC Apprentice
CNC Apprentice
Posts: 90
Joined: Tue 23 Aug , 2011 18:25 pm
Hardware/Software: Denford Triac PC. VR Milling 5.51.0.616

Re: Arc converted to straight lines.

Post by MAX THE MILLER » Fri 19 Dec , 2014 15:54 pm

No matter which boxes I tick VR Milling converts the 8 inch radius arc to four straight lines.

I'll have to try writing my own G Code.

MAX THE MILLER
CNC Apprentice
CNC Apprentice
Posts: 90
Joined: Tue 23 Aug , 2011 18:25 pm
Hardware/Software: Denford Triac PC. VR Milling 5.51.0.616

Re: Arc converted to straight lines.

Post by MAX THE MILLER » Tue 23 Dec , 2014 15:34 pm

In the end I wrote my own G Code for the part using tool offsets and arc drawing commands. The actual cutting part is only about five lines which is far less than VR Milling produced when importing the DWG file. The part was successfully cut and has a nice smooth arc.

TDIPower
CNC Guru
CNC Guru
Posts: 398
Joined: Tue 29 Apr , 2014 18:38 pm
Hardware/Software: Starturn 5 (sort of running, I will get this done!)
Lathe cam designer V1.11
Quickturn 2D Design
FANUC offline and online programs.
Microrouter Pro NS V5 (microstep)
VR2 and VR5
Boxford VMC260
Techsoft 2d Design tools V1 > V2
ProDesktop
Fusion 360
Deskproto

Re: Arc converted to straight lines.

Post by TDIPower » Tue 23 Dec , 2014 21:26 pm

At least you got the job done. Very frustrating when the software should do it though.
Just had a thought. As I have access to Deskproto you could send the drawing to me and I could see how that produces the code. I could also have a go at drawing it on 2D Design tools and see how VR5 converts it. I could send the code files back so you could look to see what they are doing.

Pete

MAX THE MILLER
CNC Apprentice
CNC Apprentice
Posts: 90
Joined: Tue 23 Aug , 2011 18:25 pm
Hardware/Software: Denford Triac PC. VR Milling 5.51.0.616

Re: Arc converted to straight lines.

Post by MAX THE MILLER » Tue 23 Dec , 2014 23:05 pm

You'll find DWG and DXF files in the first post in this thread. Most drawing packages should open these.

Dimensions aren't shown, but are embedded in the files so you should be able to add them. Dimensions are metric.

It'd be interesting to see whether another CAM package does a better job of producing the G Code than VR Milling does..

TDIPower
CNC Guru
CNC Guru
Posts: 398
Joined: Tue 29 Apr , 2014 18:38 pm
Hardware/Software: Starturn 5 (sort of running, I will get this done!)
Lathe cam designer V1.11
Quickturn 2D Design
FANUC offline and online programs.
Microrouter Pro NS V5 (microstep)
VR2 and VR5
Boxford VMC260
Techsoft 2d Design tools V1 > V2
ProDesktop
Fusion 360
Deskproto

Re: Arc converted to straight lines.

Post by TDIPower » Wed 24 Dec , 2014 0:10 am

Ive just imported the DXF into 2D design tools,

the long straight edge is 71.44mm
the shorter edges are 17.46mm
the radius of the curve is 203.2mm

Now importing the DXF into Prodesktop 8 (3D cad program)

the long straight edge is 71.43mm
the shorter edges are 17.46mm
however the radius is showing up as a radius of 203.2mm when I add a dimension to it BUT looks like 4 straight lines on the screen.

Ill need to fire up another PC which has Deskproto on. Ill try and get chance tomorrow. I know it will do files for the micromill but not sure about the triac.
could you let me know the cutter specs, depth of cut and material. Is the centre of the cutter to follow the path or offset in/outside of the line?

Ive attached 2 DXF files, when I went to export from 2D design tools it gave me the option to use arc or not use arc command.
Attachments
cp no arc.dxf
Use Arc not selected
(5.56 KiB) Downloaded 392 times
CP Arc.dxf
Use Arc selected
(3.33 KiB) Downloaded 405 times

MAX THE MILLER
CNC Apprentice
CNC Apprentice
Posts: 90
Joined: Tue 23 Aug , 2011 18:25 pm
Hardware/Software: Denford Triac PC. VR Milling 5.51.0.616

Re: Arc converted to straight lines.

Post by MAX THE MILLER » Wed 24 Dec , 2014 11:18 am

Hello and thanks for your efforts.

The odd dimensions are down to the original paper drawing having fractional imperial dimensions. I redrew it using imperial decimal dimensions. The curve at the top has a radius of 8 inches. I convert all imperial drawings to metric before importing them into VR Milling. This is because VR Milling can't handle imperial files when it comes to drilling holes. This is the subject of another thread and is awaiting a solution from Denford.

The full drawing process is this:-

1. Original paper drawing redrawn with imperial decimal dimensions using AutoSketch which uses its own .skf file extension.
2. Autosketch drawing changed to metric dimensions.
3. Autosketch drawing saved with a .DWG file extension and imported into VR Milling.

Material used is brass. Cutter used was 3mm diameter slot drill. Depth of cut was 1.5mm done as 3 times 0.5mm cuts. Cutter to be offset to outside of drawn line.

It's probably not worth your devoting much time to this as I have successfully made the part.

What I'm really interested in is whether the problem is down to the drawing or VR milling. The only way to prove this either way would be to redraw the part using another drawing package, import it into VR Milling and inspect the resulting decode or run a simulation.

TDIPower
CNC Guru
CNC Guru
Posts: 398
Joined: Tue 29 Apr , 2014 18:38 pm
Hardware/Software: Starturn 5 (sort of running, I will get this done!)
Lathe cam designer V1.11
Quickturn 2D Design
FANUC offline and online programs.
Microrouter Pro NS V5 (microstep)
VR2 and VR5
Boxford VMC260
Techsoft 2d Design tools V1 > V2
ProDesktop
Fusion 360
Deskproto

Re: Arc converted to straight lines.

Post by TDIPower » Wed 24 Dec , 2014 18:48 pm

Try those 2 files I created in Techsoft 2D designtools. I drew them in metric from the dimensions I got from adding dims to your drawings.
one is with using the arc command on export the other without.

I saw your post about the inch issue as well.

Im interested to find out what the occurrence is in case I run into it in the future. 2d stuff I do on Techsoft so if that is ok for you I know where I stand.

Cheers

Pete

MAX THE MILLER
CNC Apprentice
CNC Apprentice
Posts: 90
Joined: Tue 23 Aug , 2011 18:25 pm
Hardware/Software: Denford Triac PC. VR Milling 5.51.0.616

Re: Arc converted to straight lines.

Post by MAX THE MILLER » Wed 31 Dec , 2014 15:44 pm

I have tried both your files, running them in 2D simulation and manually checking the GCode. In both cases the arc is reduced to four straight lines.

Tried some experiments and found that VR Milling works OK when cutting for example an 8" radius semi circle. It uses G2 instructions to do this, producing a perfect arc.

The problem comes when trying to cut an arc whose radius and length make it come close to becoming a straight line. It is then reduced to a series of straight lines, but not enough lines to resemble an arc.

Trouble is I can't work out where the change from a true arc to a series of straight lines occurs. It appears to be a function of arc length (or angle) versus arc radius.

I'm going to have to exercise caution when cutting large radius arcs, checking the GCode first, to avoid wasting material.

Gazah
Posts: 4
Joined: Sat 05 May , 2012 3:10 am
Hardware/Software: Triac pc

Re: Arc converted to straight lines.

Post by Gazah » Fri 09 Oct , 2015 0:50 am

Even with the latest version of VR Milling 5.61 there is a serious problem with arc's being converted in to a series of steps with a cutter over 6mm
I have gone back to version 5.53 because it does not suffer from this fault
I wish Denford would sort this issue out

MAX THE MILLER
CNC Apprentice
CNC Apprentice
Posts: 90
Joined: Tue 23 Aug , 2011 18:25 pm
Hardware/Software: Denford Triac PC. VR Milling 5.51.0.616

Re: Arc converted to straight lines.

Post by MAX THE MILLER » Fri 09 Oct , 2015 12:58 pm

I wish Denford would sort this out too.

I also wish they'd sort out the problem with drilling holes when importing an imperially dimensioned drawings which has been outstanding for nearly three years.

viewtopic.php?f=2&t=3903&hilit=DRILLING+HOLES

VR Milling 5 is a product for which I've bought a licence, not a freebie.

User avatar
Denford Admin
Site Admin
Posts: 3588
Joined: Fri 10 Feb , 2006 12:40 pm
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.
Location: Sunny Brighouse
Contact:

Re: Arc converted to straight lines.

Post by Denford Admin » Wed 14 Oct , 2015 12:11 pm

Hi. VR Milling converts the shallow arc into four lines. It needs to do this for the path calculations.

We've tried the same DXF file with Quickcam 2D and the file is then imported as an arc. Do you have an installation of Quickcam to import the DXF file, and then send the produced fnc file to VR Milling? Alternatively is it possible to explode the arc into a more detailed poly line in AutoSketch and then import the DXF file?

Does Quickcam also have the same issue with imperial drill holes?

MAX THE MILLER
CNC Apprentice
CNC Apprentice
Posts: 90
Joined: Tue 23 Aug , 2011 18:25 pm
Hardware/Software: Denford Triac PC. VR Milling 5.51.0.616

Re: Arc converted to straight lines.

Post by MAX THE MILLER » Fri 16 Oct , 2015 16:25 pm

It's good to see that Denford are taking an interest in this problem.

I don't have a copy of QuickCAM 2D, but as far as I can see this problem is present regardless of the drawing package used.

In the Autosketch DXF file the arc is clearly specified as an arc, not a series of arcs, series of straight lines or a polyline. If I specify an arc I expect an arc to be cut, not a series of straight lines.

I cannot see why VR Milling has to convert shallow arcs to four straight lines in order to plot paths. The machine's hardware, electronics and firmware are perfectly capable of cutting a shallow arc if fed with the correct G2 or G3 instruction. Indeed I was able to cut the part in question by writing my own G Code, which I've attached.

If I am to follow your suggestion of specifying a shallow arc as a series of arcs or a polyline I'd need to know at what point VR Milling decides an arc is shallow. Not really a practical proposition.

I don't think the hole drilling problem is anything to do with the drawing package either. As Denford have stated:-

"I can see the problem here.

It appears that the hole positions are not being scaled when you pick the drill plan.(everything should be scaled to metric units)

Can you set the original CAD system to output Metric units ? That will probably fix the problem while we sort it out in VR Milling".

At least with the hole drilling problem I can see that things are going wrong as soon as I import the file. I then have to go back to the imported file and convert it to metric dimensions before trying again. At least no material is wasted.

With the shallow arc problem I have to run a simulation or go through the G Code to see whether the arcs are going to be cut correctly as an arc or as four straight lines. Not good where a part has many arcs.
Attachments
arc properties.txt
(341 Bytes) Downloaded 546 times
Project Coal Plate.fnc
(597 Bytes) Downloaded 376 times

User avatar
Steve
CNC Guru
CNC Guru
Posts: 1261
Joined: Tue 21 Feb , 2006 16:15 pm
Location: Denford UK

Re: Arc converted to straight lines.

Post by Steve » Mon 19 Oct , 2015 9:41 am

The DXF import into VR Milling was added to help people use the software with External CAD packages. We used a CAD engine piece of software purchased in 2004 to do this and that engine is no longer supported. Where newer formats of DXF have been developed this can cause a problem. We have limited control as to how we can handle this function. Even if the DXF contains ark data we have to then extract that data and create new paths within the software to generate the cutter paths. Generally we break down the lines into a series of points to do this.

The DXF import has gone through several changes as we try to resolve issues for customers. The problem can be that fixing one customers issue can then cause problems for another and as we are unable to make changes in the CAD engine we are restricted to what we can do.

Do you have any option in your cad package to save in EPS format? In some cases the CAD packages output a better EPS file than DXF?

If you could explode your CAD Drawing before exporting this could also help.

We will try an make some fixes for this problem.

MAX THE MILLER
CNC Apprentice
CNC Apprentice
Posts: 90
Joined: Tue 23 Aug , 2011 18:25 pm
Hardware/Software: Denford Triac PC. VR Milling 5.51.0.616

Re: Arc converted to straight lines.

Post by MAX THE MILLER » Sun 25 Oct , 2015 16:55 pm

Auto Sketch can create .eps files, but I can't find a way of importing them into VR Milling. The VR Milling help file only mentions importing .dxf and .dwg files.

Auto sketch won't allow the .dxf file to be exploded.

I notice that the way VR Milling handles arcs has changed during the time I've been using the product. With regards to the .dxf file attached to an earlier post:-

Ver 5.51 cuts about 200 straight lines. Probably gives a good arc, but it's difficult to see what's going to happen by looking at the Gcode.
Ver 5,54 cuts a single straight line.
Ver 5.61 cuts 4 straight lines.
Attachments
EXPLODE.jpg
EXPLODE.jpg (126.41 KiB) Viewed 9970 times

Gazah
Posts: 4
Joined: Sat 05 May , 2012 3:10 am
Hardware/Software: Triac pc

Re: Arc converted to straight lines.

Post by Gazah » Mon 26 Oct , 2015 2:02 am

Until Denford sort this issue out I have gone back to version 5.53
There is not a problem with this version it works fine with DFX import
Same cad package that works with version 5.53 does not work with the new versions
You can see there is a problem if you tick the convert polylines to arcs by the number of lines of code produced
My one DFX file produces nearly 700 lines of code in version 5.53 with convert polylines to arcs unticked and about 70 with it ticked
In the later versions it will not output more than 130 with convert polylines to arcs unticked and the finish is rubbish
It's even worse with it ticked
This makes the later versions of the program unusable for me !!!

Post Reply