Inlay Tool

This forum is for general discussion regarding VCarve Pro
Post Reply
stevenW
Posts: 5
Joined: Fri Nov 24, 2017 2:18 am
Model of CNC Machine: X-carve 750X750

Inlay Tool

Post by stevenW »

I am having problems with the inlay tool. I have used it successfully with shapes and small lettering. However, I am making a monogramed cutting board with a large G in the center. I am trying to use the inlay tool but the male insert is coming out much too large. I am keeping both allowances at 0.

Here is a picture with a test board. The Male inlay is on the left and the female pocket is on the left. You can see that there is no way the insert will fit.
inlay tool.jpg
Any suggestions will help.

Steven

User avatar
martin54
Vectric Archimage
Posts: 7339
Joined: Fri Nov 09, 2012 2:12 pm
Model of CNC Machine: Gerber 48, Triac PC, Isel fixed gantry
Location: Kirkcaldy, Scotland

Re: Inlay Tool

Post by martin54 »

Are you sure the male G is far to large to fit ? Have you actually measured to make sure it won't fit ? If you are using the same vector for both then there shouldn't be a problem. Are you sure it isn't just a trick of the eye ?? :lol: :lol:

Bob Reda
Vectric Wizard
Posts: 858
Joined: Wed Aug 16, 2006 7:34 pm
Model of CNC Machine: shopbot 48x48 upgraded prt
Location: Monessen, Pa
Contact:

Re: Inlay Tool

Post by Bob Reda »

You also must use the same tool for both or the radius will be different

Bob

User avatar
Adrian
Vectric Archimage
Posts: 14547
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: Inlay Tool

Post by Adrian »

It doesn't look like the pocket has cut correctly to me. The corners aren't shaped correctly. Perhaps you're pushing too hard.

stevenW
Posts: 5
Joined: Fri Nov 24, 2017 2:18 am
Model of CNC Machine: X-carve 750X750

Re: Inlay Tool

Post by stevenW »

I used the same vector and bit size for both. the tool path presentation for both were correct. its just when i actually carved them that the problem with the oversized male inlay occurs.i tried 3 times with actual carvings. the graphic was an attempt to show both for comparison. i stopped the pocket before it was 100% complete which resulted in the shaper edge. however the over all outline size was complete.

User avatar
martin54
Vectric Archimage
Posts: 7339
Joined: Fri Nov 09, 2012 2:12 pm
Model of CNC Machine: Gerber 48, Triac PC, Isel fixed gantry
Location: Kirkcaldy, Scotland

Re: Inlay Tool

Post by martin54 »

How far is it away from fitting ??
If you have both allowances at zero then it will never fit (unless its a fluke), you need some allowance for one part to sit inside the other, you also need a little bit of room for glue :lol: :lol:
I always cut the male part first, then when I cut the pocket if the male part doesn't fit you can increase the allowance & run the toolpath again, had to do this 2 or 3 times on occasions :lol:

Have you measured the inlay & the pocket to see just how far out it really is ??

User avatar
mtylerfl
Vectric Archimage
Posts: 5865
Joined: Thu Jan 29, 2009 3:54 am
Model of CNC Machine: -CarveWright CNC -ShopBot Buddy PRSAlpha
Location: Brunswick, GA

Re: Inlay Tool

Post by mtylerfl »

Hi Steven,

Go ahead and post the file so we can see and pinpoint any errors in the layout for you (besides the zero tolerance error that Martin already alerted you to).
Michael Tyler

facebook.com/carvebuddy

-CarveWright CNC
-ShopBot Buddy PRSAlpha CNC

stevenW
Posts: 5
Joined: Fri Nov 24, 2017 2:18 am
Model of CNC Machine: X-carve 750X750

Re: Inlay Tool

Post by stevenW »

Here is the gcode for both pocket and insert of the original letter G that I am trying to inlay. The graphic shows what vcarve thinks its going to carve. The size of the insert is matched to the pocket. Once carved the insert is about 1/8 in tool large at the large left arch with the remaining area of the G about 1/16 too large. I tried using the pocket allowance but to make it sort of fit the pocket was starting to become misshapen.
Pocket Inlay 1.txt[/p] [attachment=0]Toolpath.jpg
Attachments
Male Inlay 1.txt
(21.2 KiB) Downloaded 183 times
Pocket Inlay 1.txt
(43.19 KiB) Downloaded 139 times
Toolpath.jpg

KeithW
Vectric Craftsman
Posts: 118
Joined: Sun Jun 08, 2014 3:13 am
Model of CNC Machine: Probotix Meteor, Aspire 8.014
Location: Red Deer, AB

Re: Inlay Tool

Post by KeithW »

You need to cut the male as a mirror image, or it won't ever fit..., unless you're just going for a straight pocket inlay.

.2 depth on the female side, .1 start depth with a .1 cut depth, and it should fit. I have good luck with a 60 deg bit, some use a 30 deg for finer detail. 60 would work on those letters.

stevenW
Posts: 5
Joined: Fri Nov 24, 2017 2:18 am
Model of CNC Machine: X-carve 750X750

Re: Inlay Tool

Post by stevenW »

I tried another Inlay Tool project and the exact thing happened, the insert was too large to fit the pocket. I had to use a pocket allowance of -.054 to force the insert in. Notice in the graphic the with an allowance of -.054 it over cut some areas and under cut others. Also, I purchased my xcarve in May and have not been able to create a vcarve yet, using vcarve, as I get the same issue. The male insert is proportionally too large to fit the vcarve pocket. I don't know if its the xcontroller or the vcarve software generated gcode.

I used the same 1/8 end mill and vector for the project.
thumbnail.jpg

User avatar
IslaWW
Vectric Wizard
Posts: 1402
Joined: Wed Nov 21, 2007 11:42 pm
Model of CNC Machine: CNC Controller Upgrades
Location: Bergland, MI, USA

Re: Inlay Tool

Post by IslaWW »

Can I assume that you were using climb mill direction for your cuts? These have been the defaults in Vectric software for over 10 years. :oops:

Try this: Set direction to conventional, recalculate and post the results. It is really that simple
Gary Campbell
GCnC Control
ATC & Servo Controller Controller Upgrades
GCnC411 (at) gmail.com

User avatar
FixitMike
Vectric Wizard
Posts: 2173
Joined: Sun Apr 17, 2011 5:21 am
Model of CNC Machine: Shark Pro Plus (retired)
Location: Burien, WA USA

Re: Inlay Tool

Post by FixitMike »

1/8" end mills bend under load. Especially when climb milling. I'm not surprised that the inlay is 1/16" too large. That's only 1/32" on each side. Also, there is machine deflection.

Actually, all end mills bend under load. Of course the amount is much less for larger ones. No one worries about .0001" deflection in a 1/2" dia. cutter when cutting wood.
Good judgement comes from experience.
Experience comes from bad judgement.

User avatar
IslaWW
Vectric Wizard
Posts: 1402
Joined: Wed Nov 21, 2007 11:42 pm
Model of CNC Machine: CNC Controller Upgrades
Location: Bergland, MI, USA

Re: Inlay Tool

Post by IslaWW »

Mike is right. That said most endmills don't bend (or deflect) as much as many people think they do. A quarter inch solid carbide bit will deflect around .007" before it breaks. An eighth a little more.

Most deflection (deviation from the actual vector) is in the machine components. Technically noted as "failure of the machine to withstand the cutting force"

Inlays, i.e., cutting a part that is required to fit tightly into another cut amplifies all of the issues. The issue that affect accuracy are:

See below
Accuracy.JPG
Gary Campbell
GCnC Control
ATC & Servo Controller Controller Upgrades
GCnC411 (at) gmail.com

User avatar
martin54
Vectric Archimage
Posts: 7339
Joined: Fri Nov 09, 2012 2:12 pm
Model of CNC Machine: Gerber 48, Triac PC, Isel fixed gantry
Location: Kirkcaldy, Scotland

Re: Inlay Tool

Post by martin54 »

What speed & feed settings are you using, posting the actual .crv file would allow some of the board experts to help more.

How much time did you spend setting up your machine to cut accurately & to determine what speed, feed & DOC settings your machine was actually capable of ??

You have mentioned that you don't know if the problem is with the controller or the generated gcode but you have overlooked the possibility as Adrian has already said that you are simply trying to push the machine to hard :lol: :lol:

You have purchased a machine that from what I have read & can see is not very rigid, doesn't mean it can't do this sort of work but it does mean that you have to make allowances for these things. Try cutting the pocket a few times using different speed, feed & DOC settings & compare the results :lol: :lol:

As IslaWW has pointed out there are a lot of variables to consider :lol: :lol:

stevenW
Posts: 5
Joined: Fri Nov 24, 2017 2:18 am
Model of CNC Machine: X-carve 750X750

Re: Inlay Tool

Post by stevenW »

I'm going to perform the alignment test using the test patteren on the inventable site.

here is the finished cutting board. I was able to work around the gaps shown in the previous picture.
15147598386691792206569.jpg
Steven

Post Reply