automatic round-overs?

Discussion/questions about software used with your CNC Shark and programming issues

Moderators: al wolford, sbk, Bob, Kayvon

Post Reply
usd294
Posts: 7
Joined: Tue Mar 26, 2013 11:10 am

automatic round-overs?

Post by usd294 »

hi, i am a studentt at high school learning how to use the cnc machine(shark pro) and while tttrtying to make a insert with 3" verdana letters using vetric VCarve Pro 6.5 and on corners of the letters it would round over mor than the 1/8 endmill, when i asked about tttthis on vetrics forum they said to ask here abouttt the cnc machine automatically rounding over

any help would be appreciated, thanks


tps ttthis computers t key sometimes shoots of extereta ttt's:)

drueth
Posts: 208
Joined: Sat Jul 09, 2011 7:09 am

Re: automatic round-overs?

Post by drueth »

usd294

There are at least two way that a user can do a inlay with Vcarve Pro . One is using a V Bit an using a V-Carve tool path. The other is using and EM and a Create Inlay Toolpath. As far as the Shark "automatically rounding over" There is no such thing. There is and always will be the problem and it is on all CNC machines that you can not cut a sharp inside corner with a round bit. If that is what your problem is look into the Inlay toolpath There are also good training film's on the Vectric site that will explane both ways. It alway help if you post some pic. of the problem so someone can have a better idea what you are trying to do. One other thing that will cause you a problem with any inlay. You must use the same bit to do the male and female cut. AND you need to be sure of the bit diam. or angle. Most 90 deg V bits are really close to 85 deg's Most 0.25 EM are abot 0.23 so you need to make a test cut to check out the bit you are using .
drueth
Shark Pro Plus HD
new to CNC 12/2012

usd294
Posts: 7
Joined: Tue Mar 26, 2013 11:10 am

Re: automatic round-overs?

Post by usd294 »

ittt is rounded far to much for a 1/8 end mill i. e. 1/4 radius, and i would postt pictures but the shop was cleaned and it was thrown awaty, i will run another cut and try to have something up tomorrow, we have ordered a few finer bits, but 1/8 end-mill is the finestt we have rightt now , i will ask onthe vetric forum again

thepuchman
Posts: 47
Joined: Tue Feb 28, 2012 7:01 am
Location: Bridgeport, IL

Re: automatic round-overs?

Post by thepuchman »

Not sure I completely understand the problem but it could be the ramp entry/exit for the tool. The value maybe too large or possibly need to omit the ramp and use a plunge entry.

adowty
Posts: 21
Joined: Tue Jul 24, 2012 5:21 pm

Re: automatic round-overs?

Post by adowty »

Hey there,

I have had this problem.
when I make a rectangular pocket path, three of the corners are WAY rounded off while the fourth is the radius of the bit.
when I make a simple profile of straight line channel, the machine runs down the straight line, then lifts prematurely at the end causing a ramp-up.
It would help the big guys here, if you have time, to make a video of the machine cutting and submit a file.
(I never had time)

My solutions:
I actually made my rectangular pocket path with rounded corners the size of my bit.
I added drill path to clean out the end of my straight channel path.

Likewise, you could add drill paths to all the little corners of your typeface. Naturally, you shouldn't have to do this, but...

I never have these kinds of problems when I export from cut3d, only the 2d software. Shark Pro Plus HD.

Good luck.

adowty

User avatar
Consultingwoodworker
Posts: 333
Joined: Fri Jul 02, 2010 7:37 am
Location: Nashville area
Contact:

Re: automatic round-overs?

Post by Consultingwoodworker »

Usd294,

If you want to send me your VCarve file (.crv) and your G-Code file (.tap) for this project, I will be happy to look them over and see if I can figure out your issue.

The Shark is NOT rounding those corners itself unless there is a mechanical fault, and if there is it is HIGHLY unlikely to be repeatable.

I can read the G-Code and compare it to the VCarve program to find where the problem lies. Send them to: rbagnall@consultingwoodworker.com

You should also try doing the inlay "manually". I inlaid a map of the islands of Venice. I did NOT use the inlay tool in VCarve, I simply pocketed the vectors in one program, and cut the same vectors in a second program as a profile.

You DO need to make the inlay smaller than the pocket, over 20 years of programming I have found that 0.014" is about right. To minimize distortion, offset the pocket cut outward by 0.007" and the inlay inward by the same.

You will also need to manually round over any sharp points on your inlay to match the bit diameter, but this is easily done. I typically use DeltaCad for drawing then import the .dxf.

Last tip on inlays: I use a 1/16" or 1/32" ball end carving bit for both the pocket and inlay. This bit is tapered so it creates a slight angle on the wall of the pocket. Invert the inlay cut out and you get a matching angle on the inlay. The inlay then can be set into the pocket like a plug, and the slight "scarf" joint around the edges looks much cleaner than a straight butt joint.

Ralph

jeb2cav
Site Admin
Posts: 1524
Joined: Thu Sep 30, 2010 7:04 pm
Location: Kentucky
Contact:

Re: automatic round-overs?

Post by jeb2cav »

An additional comment on this - the Shark post processor does have a G64 command in it. If everything else about your setup is 'correct' - nothing loose, all is mechanically sound - and you require extreme precision, then remove that line from the post. Even the USB Arc Inch can result in the resulting cut travelling 0.01" away from the toolpath vector. In many cases, this is acceptable. In some, it is not - beauty is in the eye of the beholder and the requirements at hand.

Post Reply