MDF Shaker Style 1 piece cabinet doors

[cusoak]

I have want to make a shaker style 1 piece Kitchen cabinet door.
I have attached a file that I did to create the the door.
The inside edge of each of the door tops sides and bottom have a bevel on them
Could you take a look at my file and see if I have created it properly and that I am going to have sharp in side corners.
Thanks Jeff Peters

Mdf Door.crv

(81 KiB) Downloaded 215 times

[martin54]

How does it look in the toolpath preview? If that shows sharp inside corners then that's what you will get if you set everything up correctly
Looks like you may have in the attachment, don't have the software on this machine so can't check the file.

dealguy11 is your man for this sort of thing so he will be able to tell you the best way to make cabinet doors I am sure

[Adrian]

As Martin says what you see is what you get. The preview for that file shows sharp corners so that's what you'll get.

You may want to check your profile toolpath for the line as you've currently got it set for inside/left rather than being On the line so it doesn't line up with the corner.

I don't know what your machine is capable of but the pass depths look very conservative to me especially for MDF.

[dealguy11]

I make a lot of MDF doors. There are a couple of things I'd do differently:

1. I would generally not use a v-carve path for this kind of door, because I don't want the v-carve bit to waste time in the corners, and I don't want to sand out the ridges it leaves. Instead, I'd pocket out the center with a 2 or 3- bit sequence, using a pocketing toolpath, starting with the large tool and ending with a 1/8" end mill. I would set up the 1/8" end mill to cut in 1 or 2 passes at most, since the large tool will have hogged out most of the material. On the doors I do, I start with a 1 1/4" pocketing bit, followed by a 1/2" end mill (which only goes around the edges), followed by the 1/8" end mill (which also only goes around the edges. This will also avoid the little ridges left by the v-bit. I follow this with a profile cut using the v-bit. You do need to define one more vector to do this. It has to be offset out from the vector used for hogging out the center. If you're using a 90-degree bit, then it needs to be offset by .375" (i.e., exactly the depth of the center pocket). The v-bit is set to cut inside the vector, .375" cutting depth, and you have to use the "Corners" tab on the profile toolpath, checking "Sharp Internal Corners (3D)". This tab will only appear if you have "Show advanced toolpath options" checked at the top of the profile toolpath dialog.

2. I don't like to use an offset style path that goes round and round when I hog out the material in the middle. This leaves diagonal witness marks at the corners that I feel are harder to sand out. I always use a raster style for these pockets.

3. For the fake seams, I agree with Adrian that they should cut on the line.

4. I'm guessing the the feeds and speeds will be limited by what your machine can achieve. MDF doors will highlight any misalignment or movement in your machine...you will quickly find out how stiff and accurate it is. Push it up on the larger bits until you start getting bad results, then step back a little.

5. Make sure you're using really good MDF. The stuff from the box stores will disappoint you. It's too fluffy in the center to cut cleanly or paint well. See if you can find Weyerhauser Glacier Green, or Trupan double refined.

6. After you cut it, only sand with higher-grit sandpaper (220 or 320) to avoid opening up the material even more than it already is. You'll need to seal it with a high-solids primer in order to get a good result. It will take 2 coats of primer, scuffing heavily after the first coat to get rid of fuzzies. Then top coat.

Good luck!

[cusoak]

Steve, Thanks for the reply, Would you be willing to take my door file and and set up the toolpaths that you would use My largest pocketing is only 1 "in dia but I have all the other bits sizes you recommend.
This is going to be my first attempt at doing something like this.
thanks Jeff

[dealguy11]

See attached. New toolpaths are in the group "Alternative toolpaths". Notes:
1. I ended up offsetting your inner frame vector in, not out, and using the new vector for the pocket. This maintains your rail and stile width.
2. I set up the 1/8 end mill as a profile path, not part of the pocket path, to avoid cleanout triangles in the corners that are not needed. I could have instead created little 0.2 x 0.2 squares at each corner run a profile path inside the squares to save a little time, but you have to be very confident that all the bits are the stated diameter and also it's more hassle to set up.

You need to check all the speeds and feeds and also adjust the tool numbers for your machine. I left them as I use them on my machine, which is a very different CNC than yours. Also make sure your tool measuring approach is accurate to avoid height artifacts when you change bits. I measure everything from the table for consistency.

There are more toolpaths here, but it should result in a cleaner product that is easier to sand & finish.

[cusoak]

Steve Thank you very much for doing this. I really appreciate
Jeff

[cusoak]

Steve i can not open the file to change the check the feeds and or make changes
I thought you would send my a vectric design file
Jeff

[Adrian]

Steve i can not open the file to change the check the feeds and or make changes
I thought you would send my a vectric design file
Jeff

He posted the file in Aspire format rather than VCarve format. Here's the same file but in VCarve format so you can get going with it.

[dealguy11]

My apologies. Forgot which forum I was on.

[cusoak]

Thanks for posting the v carve file I is just what I I wanted
I always get great help here.
Jeff

[cusoak]

Steve I checked the feed rates and with my Shapeoko with a DEWALT 611 router which limits me to 1/4' and 1/8" shank bits
Which I believe were not supposed run at 400 inches ipm So I will need to do some adjusting .
Thanks Jeff

[cusoak]

one last question .when saving the toolpaths created for the pocket with 3 different bits do I out put them to 1 toolpath or so I do them separately
I do not have a tool changer.
Jeff

[dealguy11]

Depends on your machine controller. On some machines with no automatic tool changer, outputting to an ATC post-processor will cause the machine to stop and wait for a tool measure between toolpaths. Other machines don't support that. I don't know how your controller works, so safest is to output to 3 files.

[cusoak]

Thanks for the reply there is a ATC processor for my Shapeoko I found so now I need to install it. And my controler will then pause and will stop for a tool change then it will go to what is called a bit setter to reset the z height for that bit then run the toolpath for that bit.
Thanks Jeff