Uneven depth of profile cut when cutting out shapes

Post general information and questions relating to Cut2D in this Forum.

Uneven depth of profile cut when cutting out shapes

Postby mplsartist » Sat Feb 03, 2018 10:25 pm

I'm cutting out shapes from 3/4" Baltic Birch (with a black laminate on the face) for my sculptures, and getting uneven depth of profile cuts from one side of each piece to the other. The strange thing is that the right side of each piece being cut is cut too shallow, requiring me to manually finish the cuts with a hand held Dremel Tool. The spoilboard has been leveled. The gantry is level to the spoil board. The collet of the router is also level to the spoil board.

If the gantry or spoil board were not level, then I would imagine that all the cuts would gradually get deeper as they moved across the board. If the collet was out of level, then I would imagine that the router bit would cut unevenly all the way around each piece with one edge being shallow and the other edge deep.


I'm using the OOZnest 1500x1500 with a Dewalt 611 router, Whiteside 1/4" spiral up cut bit. I'm using Vectric Cut2D Pro with the following settings:
Board thickness: 0.714
Start depth: 0.025
Total thickness entered: 0.739
Total cut depth entered: 0.739
Individual pass depth: 0.0616
Total passes: 12
Conventional cut
Feed rate: 80 ipm
Allowance offset: 0.04
Separate last pass
No reverse direction
No allowance
3D tab thickness: 0.125
3D tab length: 0.35

I've attached a photo so that you can get a better idea of the problem. Any ideas?
Shallow Right Side cuts.jpg
Last edited by mplsartist on Sat Feb 03, 2018 10:45 pm, edited 1 time in total.
mplsartist
 
Posts: 27
Joined: Thu May 25, 2017 2:09 pm
Model of CNC Machine: OOZnest 1500x1500

Re: Uneven depth of profile cut when cutting out shapes

Postby mtylerfl » Sat Feb 03, 2018 10:41 pm

Not sure why you entered a different thickness for your material. Enter the true material thickness (0.714") and enter the Cut depth (0.739") as the larger amount only.

Also not sure why the Starting Depth is set at 0.025" for your cutout. That will give you a total depth of 0.764". If that's what you want, just enter that and have a zero Start Depth.

You said you surfaced your spoilboard, but are you certain your router is perfectly perpendicular to the spoilboard surface in both x and y?
Michael Tyler

carvebuddy.com

facebook.com/carvebuddy

-CarveWright CNC
-ShopBot Buddy PRSAlpha CNC
User avatar
mtylerfl
Vectric Wizard
 
Posts: 3284
Joined: Thu Jan 29, 2009 3:54 am
Location: Brunswick, GA
Model of CNC Machine: -CarveWright CNC -ShopBot Buddy PRSAlpha

Re: Uneven depth of profile cut when cutting out shapes

Postby Rcnewcomb » Sat Feb 03, 2018 10:57 pm

Are you setting Z-Zero on the top of the material, or on the spoilboard?

Since you need clean cutouts I'd recommend Z-zero on the spoilboard.
- Randall Newcomb
10 fingers in, 10 fingers out - another good day in the shop
User avatar
Rcnewcomb
Vectric Wizard
 
Posts: 3115
Joined: Fri Nov 04, 2005 5:54 am
Location: San Jose, California, USA
Model of CNC Machine: GCnC/WinCNC

Re: Uneven depth of profile cut when cutting out shapes

Postby mplsartist » Sun Feb 04, 2018 1:25 am

mtylerfl:
I forgot to mention that I'm setting the starting depth at 0.025 with a metal feeler gauge so that I get a consistent starting depth vs. touching the bit on the softer birch which tends to get routed out when the bit starts turning. When I need to cut additional pieces from the same sheet of 4'x4' wood, the starting point depth remains consistent when using the metal feeler gauge.

You bring up a good point about the level spoil board. I only checked it in the X axis when I was checking the gantry for level. I'm still trying to figure out how this would cause the cuts to be perfect on left sides of the profile cuts and shallow on the right sides. This is pretty consistent across the full width and height of the 4'x4' sheet.
mplsartist
 
Posts: 27
Joined: Thu May 25, 2017 2:09 pm
Model of CNC Machine: OOZnest 1500x1500

Re: Uneven depth of profile cut when cutting out shapes

Postby mtylerfl » Sun Feb 04, 2018 1:33 am

Ok the start Depth makes sense now (and is a good idea if you don't have a metal touch plate).

I would take Randall's suggestion and zero from the spoilboard instead of the top of material. This is more or les standard procedure when cutting sheet goods. Variance in thickness is common and unless using vac hold down, difficult to hold a 4' x 4' sheet down flat over its entire area.

Zeroing from the bottom of the material (i.e., the spoilboard surface) should eliminate your cut through problem. Don't use the feeler gauge when zeroing from the spoilboard, though...and don't specify a start depth either, of course.
Michael Tyler

carvebuddy.com

facebook.com/carvebuddy

-CarveWright CNC
-ShopBot Buddy PRSAlpha CNC
User avatar
mtylerfl
Vectric Wizard
 
Posts: 3284
Joined: Thu Jan 29, 2009 3:54 am
Location: Brunswick, GA
Model of CNC Machine: -CarveWright CNC -ShopBot Buddy PRSAlpha

Re: Uneven depth of profile cut when cutting out shapes

Postby mplsartist » Sun Feb 04, 2018 2:52 am

Michael & Randall:

I just finished re-checking my table for level. This time I used a 4' level and got quite a different result. I discovered that my table was racked due to sitting on an old, uneven basement floor. After shimming the four legs at different heights, my spoil board is now level in both x and y axis from the front to the rear and sided to side. The gantry was level but the router needed to be readjusted so that the base of the router was level in both x & y axis.

I did recently upgrade my table to a vac hold down arrangement. The suction is coming through the MDF spoil board. Initial tests demonstrated that it provided very good holding capabilities. However, I haven't been using it recently because when I did some initial cuts, I observed that there was quite a bit of chips remaining in the toolpath after the last pass and was thinking that the vacuum was preventing my dust extraction set up from fully cleaning out the toolpath. My concern was having the router go through the build up of loose chips and possibly causing a jam up and crash of the router. Any thoughts?

In the meantime, can one of you provide a bit more info about using the spoil board as zero? If I remember correctly, Vectric provides for the starting point to be either at the top or the bottom of the wood. Does it automatically account for the thickness of the wood that I specified or do I need to enter negative numbers of some sort? I'm concerned about not using the feeler gauge as I often don't cut the whole 4x4 sheet at once. The starting point height gets altered by the starting of the router bit each time I cut some new pieces. If I specify the bottom of the sheet as zero in vectric, can I add the 0.025 thickness of the feeler gauge and get the same result as Randall has suggested?

Thanks for all the help you are providing to a CNC rookie.
mplsartist
 
Posts: 27
Joined: Thu May 25, 2017 2:09 pm
Model of CNC Machine: OOZnest 1500x1500

Re: Uneven depth of profile cut when cutting out shapes

Postby mtylerfl » Sun Feb 04, 2018 3:06 am

Now that your machine is level, you will need to re-surface the spoilboard to make it truly flat before proceeding any further.

Zeroing from the spoilboard is not anything special (you may be overthinking this). No, you don't enter any negative numbers. Yes, the software compensates for the material thickness automatically, so no worries there. Just be sure you change the z-zero location (from the top surface to the bottom) via the Material Setup and recalculate the toolpaths before running your project.

No worries about the chips either - I use downcut end mills for cutouts most of the time (which tends to pack chips in the grooves). Chips remaining in the groove are no match for the router (in my case, the spindle). It doesn't care they are there and the router won't jam. BTW, using a downcut bit and allowing chips to remain in the grooves helps hold vacuum better anyway.

You don't need to use the feeler gauge. The MDF surface is plenty hard enough that you won't need to be concerned about the tip of an end mill throwing off your z measurement.

Randall, please add any additional input you think will help.
Michael Tyler

carvebuddy.com

facebook.com/carvebuddy

-CarveWright CNC
-ShopBot Buddy PRSAlpha CNC
User avatar
mtylerfl
Vectric Wizard
 
Posts: 3284
Joined: Thu Jan 29, 2009 3:54 am
Location: Brunswick, GA
Model of CNC Machine: -CarveWright CNC -ShopBot Buddy PRSAlpha

Re: Uneven depth of profile cut when cutting out shapes

Postby mplsartist » Sun Feb 04, 2018 3:55 am

Michael:
About 10 minutes after my last post, while sitting in the hot bath tub (where ideas and inspirations seem to come to me out of the blue), I realized the same thing about the spoil board. That will be the first thing I do tomorrow morning. I'll then do some test cuts using the methods you and Randall described.

Interesting comments about the down cut end mill providing material for the vac to hold down. I was previously using a compression bit (without a vac hold down) but was having trouble with it going off track and cutting through some other pieces, etc. I'll store that away for future reference.

I'll let you know how the new procedures work out.

Thanks again!
mplsartist
 
Posts: 27
Joined: Thu May 25, 2017 2:09 pm
Model of CNC Machine: OOZnest 1500x1500


Return to Cut2D - General

Who is online

Users browsing this forum: No registered users and 9 guests