two side machining error

This forum is for general discussion about Aspire

two side machining error

Postby CCWood » Mon Oct 08, 2018 9:30 pm

:?: Trying to use Aspire's two sided machining feature. My Aspire files look correct (designs line up on top & bottom) but when I cut a part one side is consistently .25" off in the x plane... If I offset one side by .25 I can get a usable part but don't think I should have to do this each time. Anyone else have this problem? Any ideas? I have tried setting my zero to both the bottom left corner and the center but still have a .25" error. Thanks in advance.
CCWood
 
Posts: 8
Joined: Thu Sep 25, 2014 3:50 am
Model of CNC Machine: Custom rebuild of Chinese machine

Re: two side machining error

Postby IslaWW » Mon Oct 08, 2018 9:42 pm

Post a sketch or your file showing how you set up your 2 sided flip operation. Then we may be able to assist you.
Gary Campbell
CNC Technology & Training
The Ultimate Woodworking Machine
GCnC411 (at) gmail.com
User avatar
IslaWW
Vectric Wizard
 
Posts: 1109
Joined: Wed Nov 21, 2007 11:42 pm
Location: Marquette, MI, USA
Model of CNC Machine: The Ultimate Woodworking Machine

Re: two side machining error

Postby CCWood » Mon Oct 08, 2018 10:04 pm

just realized I said .25"... actually should have put .125"...
CCWood
 
Posts: 8
Joined: Thu Sep 25, 2014 3:50 am
Model of CNC Machine: Custom rebuild of Chinese machine

Re: two side machining error

Postby martin54 » Mon Oct 08, 2018 10:28 pm

What registration method are you using for flipping your work piece ? I have done quite a bit of 2 sided machining & have never had a problem with alignment :lol: :lol:

Have you watched the tutorials on 2 sided machining, there are a few of them in the training section & I think there is one from one of the user group meetings but don't quote me on that :lol: :lol: :lol:
User avatar
martin54
Vectric Wizard
 
Posts: 3904
Joined: Fri Nov 09, 2012 2:12 pm
Location: Crossgates, Scotland
Model of CNC Machine: Gerber System 48 (modified)

Re: two side machining error

Postby garylmast » Mon Oct 08, 2018 11:17 pm

If you center that datum rather than the corner of the material and use a jig rather than pegs, it will probably solve your problem. If your material is a hair off from the measurements set in Aspire, you'll get the offset if you are using the corner and pegs. I've done many double-sided projects now and the offset problem was solved once I started using this procedure.

Gary
garylmast
Vectric Wizard
 
Posts: 752
Joined: Fri Oct 23, 2009 4:03 pm
Location: Sandy, Utah

Re: two side machining error

Postby mtylerfl » Mon Oct 08, 2018 11:54 pm

I always have used two dowel pegs and always have used lower-left corner for the XY Zero origin.

Never had even a smidgen of misalignment. Jigs are not necessary, as long as everything is setup properly in the file and your machine is reliable to return to the same xy origin point consistently and reliably.

Oh, material size doesn’t matter either. As long as the job will fit on it and the dowel peg holes are properly located for flipping the material over, all will be well. You can use any scrap, irregularly shaped material you want. The dowel hole alignment is the part that sets front-to-back alignment, not the material itself.

But, if you choose to use jigs, I certainly have no problem. Whatever it takes to get the job done is all that matters!
Michael Tyler

carvebuddy.com

facebook.com/carvebuddy

-CarveWright CNC
-ShopBot Buddy PRSAlpha CNC
User avatar
mtylerfl
Vectric Wizard
 
Posts: 3222
Joined: Thu Jan 29, 2009 3:54 am
Location: Brunswick, GA
Model of CNC Machine: -CarveWright CNC -ShopBot Buddy PRSAlpha

Re: two side machining error

Postby martin54 » Tue Oct 09, 2018 1:08 am

Same as Michael, bottom left & either 2 or 3 dowel pegs depending on the size of the work piece. Never had a problem doing it this way. The only way I can see you having a problem with this method is if your 2 sides are misaligned in the software. Because I have a low gantry I have on occasions had to use 2 sided machining to profile cut thick(er) piece out cutting half from each side & not even had problems doing that because the machine is pretty accurate :lol: :lol: :lol:
User avatar
martin54
Vectric Wizard
 
Posts: 3904
Joined: Fri Nov 09, 2012 2:12 pm
Location: Crossgates, Scotland
Model of CNC Machine: Gerber System 48 (modified)

Re: two side machining error

Postby highpockets » Tue Oct 09, 2018 1:20 am

If you're using dowels are your dowels symmetrical to the center of the material?
John
Maker of Chips
User avatar
highpockets
Vectric Wizard
 
Posts: 1771
Joined: Tue Jan 06, 2015 4:04 pm
Model of CNC Machine: PDJ Pilot Pro

Re: two side machining error

Postby RebeccaJ » Tue Oct 09, 2018 8:25 am

Hey There,

This video demonstrates the asymmetrical dowel hole method: https://release.vectric.com/clipart_bowl/ this is a pretty fail safe way of flipping the part over as there is only one possible that the top side can locate with the dowels of the bottom side.

I hope this helps.
Beki Jeremy
Senior Application Engineer - Vectric Ltd.
RebeccaJ
Vectric Staff
 
Posts: 138
Joined: Fri Jun 01, 2012 1:30 pm
Location: Redditch, UK
Model of CNC Machine: Various

Re: two side machining error

Postby LittleGreyMan » Tue Oct 09, 2018 8:48 am

I totally agree with Beki: always use asymmetrical dowels. When the parts allow this method, it's the simplest and more efficient poka-yoke you can imagine for flipping parts. Unless you have a specific tool for serial parts, of course.
Best regards

LGM

W7 - Aspire 8.517
LittleGreyMan
Vectric Wizard
 
Posts: 761
Joined: Fri May 15, 2015 1:10 pm
Location: France
Model of CNC Machine: 3 axis small size machine

Re: two side machining error

Postby garylmast » Tue Oct 09, 2018 1:16 pm

My double-sided projects are usually a glue-up where I trim the edges afterwards, which makes the material a fraction off from how I set it in Aspire. Or sometimes I'll just grab a piece of material setting there, but again is different than the setup. True what everybody said about the pegs and corner datum position is actuate, however, if the material size is different the corner datum position would need to be re-positioned.

When I say I do a jig, it's simply taking some scrap wood and either screwing or shooting it with brads to the spoilboard and either screwing the material to the spoilboard or to the jig. It takes seconds, which is a whole lot faster then doing the pegs. And if I forget to reset the datum (which I was my habit when using pegs) it won't be misaligned if I use the center.

Maybe if I had more patience and my memory wasn't only a few seconds long, I would do it the other way, but I like EASY. :wink: :wink: :wink:

Gary
Attachments
Capture.JPG
garylmast
Vectric Wizard
 
Posts: 752
Joined: Fri Oct 23, 2009 4:03 pm
Location: Sandy, Utah

Re: two side machining error

Postby mtylerfl » Tue Oct 09, 2018 2:00 pm

Hi Gary,

Remember, the dowel holes determine alignment, not the edge of your material.

I think where folks struggle with this concept is that they try to cut the material to an exact size so that when flipped, the XY Zero of the corner of the material lands at the same place. No - simply make sure the material is a bit Larger than necessary to fit your layout. Proper placement of the holes in your layout is the key. Making sure the material is large enough that, when flipped, the material spans enough area (or a little more) to fit the backside job.

When the material is flipped over, it does not matter whether the edge of the material corner is at the same spot as the first side! It is irrelevant, since the dowel holes take care of the front-to-back alignment.

By thinking you need to reset the XY datum position, this invites Trouble! That position should not be changed. If you do, then that will almost guarantee a misalignment.

Keep the datum position the same at all times - do not change it. Using the dowel method will always yield perfect alignment as long as you don’t defeat this alignment by changing the XY datum location.
Michael Tyler

carvebuddy.com

facebook.com/carvebuddy

-CarveWright CNC
-ShopBot Buddy PRSAlpha CNC
User avatar
mtylerfl
Vectric Wizard
 
Posts: 3222
Joined: Thu Jan 29, 2009 3:54 am
Location: Brunswick, GA
Model of CNC Machine: -CarveWright CNC -ShopBot Buddy PRSAlpha

Re: two side machining error

Postby garylmast » Tue Oct 09, 2018 2:25 pm

Hi Micheal,

As in my illustration, if I line up the pegs holes, the datum will different (if the material size is different than set in Aspire) If you're off 1/32", the backside could be off twice (1/16"). I would then have to re-position the corner datum position, where if it is in the center, I don't have to remember. When I first started doing the double sided projects after Aspires upgrade, I was constantly getting the backside misaligned because my forgetfulness to reset the XY position. I have now done several dozen double sided projects and since I started doing the jig and center positions, I have yet to have a misalignment. I also think the jig is much easier than the pegs. However, if some way of doing something is better for one person, they could stay with the way which is more comfortable to them.

After saying all that, I like to reinvent the wheel. :twisted: :twisted: :twisted: Just kidding.

Gary
garylmast
Vectric Wizard
 
Posts: 752
Joined: Fri Oct 23, 2009 4:03 pm
Location: Sandy, Utah

Re: two side machining error

Postby mtylerfl » Tue Oct 09, 2018 2:32 pm

Well, if your method is working for you, then we are both happy!
Michael Tyler

carvebuddy.com

facebook.com/carvebuddy

-CarveWright CNC
-ShopBot Buddy PRSAlpha CNC
User avatar
mtylerfl
Vectric Wizard
 
Posts: 3222
Joined: Thu Jan 29, 2009 3:54 am
Location: Brunswick, GA
Model of CNC Machine: -CarveWright CNC -ShopBot Buddy PRSAlpha

Re: two side machining error

Postby CCWood » Tue Oct 09, 2018 6:27 pm

Hi all, Thanks for the suggestions, hints and comments... I'm now on the right track (the asymmetrical dowels video was a big help). Also found that my gantry is not exactly square (which does throw in some error on the two sided stuff), so now I'll start working on the alignment issue. Again thanks to all.
Andy
CCWood
 
Posts: 8
Joined: Thu Sep 25, 2014 3:50 am
Model of CNC Machine: Custom rebuild of Chinese machine

Next

Return to Aspire - General

Who is online

Users browsing this forum: StuC and 28 guests