Two Sided Carving

This forum is for general discussion regarding VCarve Pro

Two Sided Carving

Postby Retired FF » Mon Jul 02, 2018 3:03 am

Hi, first post from a long time lurker and new CNC owner.
I have been using VCarve Pro for about 3 months now after following things on this forum for several years.
I have an extensive back round in CAD and feel I have a good grasp on the basic use of VCarve but I'm still learning the intricacies as well as the tool path aspects.
I've set up a two sided carve and having an issue with misalignment of the two sides. Before I set up the jig I'm showing here I was doing single piece carves and had the same issue on some of them. I chalked those up to my blanks not being exactly them same width as I specified in the job size in VCarve.
I created a jig on the machine to facilitate the flip and alignment of the two sides. The blank was squared and attached to the jig and then sized to get a consistent width so that when the part was flipped along the x axis and refastened things should line up. Tool paths were set up to machine a little more than half way through the blank with tabs to keep everything in place.
I'm having misalignment along the x axis sides and I can't seem to figure out why.
Attached is a picture of my jig and a closeup of the the misalignment.
Tried to upload the CRV file but it is to large, I will try to set it up for access from my drop box if that will help or I'll remove the text carvings being done and re save to make it smaller then upload.
Only other information I can provide right now that my help is that I am using MACH3 and have the current version of VCarve Pro.
Any insight would be appreciated.
4 pack jig.jpg
Jig is actually on the machine with the long side on the x axis

Misalignment.jpg
Misalignment closeup
User avatar
Retired FF
 
Posts: 3
Joined: Thu May 31, 2018 5:57 pm
Location: South Central Pennsylvania
Model of CNC Machine: CNC RP Pro 48x96

Re: Two Sided Carving

Postby martin54 » Mon Jul 02, 2018 11:13 am

Could be down to a number of things, firstly have you taken the time to properly calibrate the machine in mach3 ? Don't need to be much out for misalignment issues to show up on 2 sided work.
Have you tried using the dowel method for registration rather than a jig ?
I use jigs for lots of things but tend to stick with dowels for 2 sided work basically because it is almost impossible for me to consistently get the stock timber EXCACTLY the size I set it to be in the software. Any deviation from the set size in the software is going to result in misalignment. With the dowel method them it doesn't really matter what size your stock is at the start :lol:

Lots of the tutorials cover its use so worth checking some of them out if you haven't already but if you have been using the forum for some time you have probably been through all the tutorials :lol:
User avatar
martin54
Vectric Wizard
 
Posts: 3789
Joined: Fri Nov 09, 2012 2:12 pm
Location: Crossgates, Scotland
Model of CNC Machine: Gerber System 48 (modified)

Re: Two Sided Carving

Postby Bill_L » Mon Jul 02, 2018 12:14 pm

Use the dowel method instead of the jig or incorporate the two together. As in the attached picture, I do 4 x 8 sheets of polycarbonate which need to be spot on. I have machined .25" index holes in my spoilboard and after placing my blank on the the table I machine the same holes into the work piece. I immediately place .25" dowels in both holes, machine the back, flip it over and finish off the front. Success is predicated on how you set up your machine to begin with. My spoilboard is secured to the table and remains in position. To start I zero the XY home position with a .25" centering pin chucked in the spindle and a .25" i.d. bronze bushing that is embedded in my table. After accurately setting my XY home is when I machine the two indexing holes in the spoilboard. So before the day begins I check and adjust my home position with the centering pin and bushing and it's off the the races. My blank sheets by the way, are slightly larger than 4 x 8 but that doesn't matter. I "eyeball" center it on the spoilboard, punch the index holes and we're ready to roll. Point here is that the index hole method ignores variations in blank size.

I do however use jigs to do some double sided machining. But here again, I incorporate two index holes and create the geometry and set the XY home position based on a .25" hole in the center of the jig.

Bill
Attachments
Poly.jpg
Bill_L
Vectric Apprentice
 
Posts: 68
Joined: Tue Jan 24, 2006 11:57 am
Location: Imperial, PA USA

Re: Two Sided Carving

Postby martin54 » Mon Jul 02, 2018 12:40 pm

So before the day begins I check and adjust my home position with the centering pin and bushing and it's off the the races

Bill, just curious, is there a particular reason you use this method ? I have homing switches on all 3 axis & first thing I do once the machine is switch on is home it to ensure the machine coordinates are set correctly. My machine is an old Gerber system 48 & the homing switches for x & y were already fitted when I got it, although it now runs with other control software I kept & use the homing switches & added on for the z axis :lol: :lol:
User avatar
martin54
Vectric Wizard
 
Posts: 3789
Joined: Fri Nov 09, 2012 2:12 pm
Location: Crossgates, Scotland
Model of CNC Machine: Gerber System 48 (modified)

Re: Two Sided Carving

Postby Bill_L » Mon Jul 02, 2018 1:04 pm

Sure. I have a ShopBot and I do have prox switches to find the XY home. But since the machine is constructed out of two different types of metal and react a little differently to temperature, after the homing it might be off slightly. Sometimes .005" and sometimes .02". By micro adjusting the pin into the bushing I'm about as accurate as anyone can be. I need to hit those index holes exactly every time I go to machine one of these sheets which I don't do every day. I guess I'm a little anal about it but the holes I need to machine in the poly have a very tight tolerance to the wall of the channel that they are machined into. My routine keeps the whole process honest.

Does that give you a better understanding ... about my insane ways? :wink: :lol: :roll:
Bill_L
Vectric Apprentice
 
Posts: 68
Joined: Tue Jan 24, 2006 11:57 am
Location: Imperial, PA USA

Re: Two Sided Carving

Postby martin54 » Mon Jul 02, 2018 2:06 pm

OK so it is slightly more accurate, Leo would say its a lot more accurate :lol: :lol: ( I would have done as well when I was having to work to that sort of accuracy) :wink:
I only asked because there is always something new to learn, the method I use has always been accurate enough for what I do & will continue to be as I work mainly with wood & that sort of accuracy won't really gain me much but it is nice to know that if I ever need a more accurate method one exists :lol: :lol:
Took me a while to learn that wood is always moving & no matter how accurate I try to be the wood always seems to outwit me :oops:

I don't consider it to be insane, people do what works best for themselves & if that method gives you the confidence in your machine then its right for you.
User avatar
martin54
Vectric Wizard
 
Posts: 3789
Joined: Fri Nov 09, 2012 2:12 pm
Location: Crossgates, Scotland
Model of CNC Machine: Gerber System 48 (modified)

Re: Two Sided Carving

Postby Bill_L » Mon Jul 02, 2018 2:30 pm

Yupper. I used to do it the Navy way. Measure with a micrometer, mark it with a piece of chalk and cut it with an ax! :roll:

I've come a long way since then.

Bill
Bill_L
Vectric Apprentice
 
Posts: 68
Joined: Tue Jan 24, 2006 11:57 am
Location: Imperial, PA USA

Re: Two Sided Carving

Postby Retired FF » Mon Jul 02, 2018 5:52 pm

Thank you both for your replies.

I was thinking when I made the jig that by incorporating a first path to machine a parallel edge from the x axis side of the jig on my blank I would be setting an exact width to match what I had set in VCarve as the job size then by flipping and placing that edge against the jig should provide the alignment I need. Obviously it's not working that way. I will figure out a way to use the dowel pin location set up and see if that helps.

I have also thought about my machine setup and how it could also cause this offset. I resurfaced the pocket on my jig using a 1/2" end mill with a 90% step over to check the tramming of the spindle to the table. Using that method I did not feel any ridges that would indicate that my spindle is out in either the x or y planes.

As far as the Mach3 settings and calibration go I'm probably really out in left field on that since all I did was download the XML file from CNC Router Parts and away I went. Got some learning ahead of me on this subject.

Martin, you mentioned calibration of Mach3, is there anything I could look at right off the bat that may give me some insight on whether Mach3 is contributing to my issue.

EDIT: Yes, I have viewed tutorials on a lot subjects, both Vectric tutorials and others that I have found on the internet.
User avatar
Retired FF
 
Posts: 3
Joined: Thu May 31, 2018 5:57 pm
Location: South Central Pennsylvania
Model of CNC Machine: CNC RP Pro 48x96

Re: Two Sided Carving

Postby Retired FF » Mon Jul 16, 2018 10:23 pm

Just wanted to post and send thanks out.
I was able to set up a dowel pin flip for this job and it worked flawlessly.
I was also able to learn some more about using MACH 3 in the process.
User avatar
Retired FF
 
Posts: 3
Joined: Thu May 31, 2018 5:57 pm
Location: South Central Pennsylvania
Model of CNC Machine: CNC RP Pro 48x96

Re: Two Sided Carving

Postby tomgardiner » Tue Jul 17, 2018 12:50 am

A note about jigs: I use jigs frequently on my table to hold blanks in small production setups. I have some that I bolt to the table where the tolerance of the part is not critical, say. 010". But when parts have to be right on within a few thousandths then I make throw away jigs from scrap mdf or particleboard screwed to the spoilboard. The jig is a pocket or hole to accept the blank machined at the time of the run. This way the jig is exactly in position for the rest of the job. The jig toolpath is drawn in the same file as the associated toolpaths so everything corresponds. After the run I pitch the jig. I keep offcuts of board on hand for fixturing..
tomgardiner
Vectric Craftsman
 
Posts: 273
Joined: Thu Oct 02, 2014 1:49 pm
Model of CNC Machine: FMT Patriot 4 x8


Return to VCarve - General

Who is online

Users browsing this forum: No registered users and 27 guests