Help drilling a grid on an angle

[Mayo]

If anyone could advise me how to do this - I know it must have a simple solution and I'm not good at manually coding files or math beyond the basics. To me, trig or calculus are like a foreign language.

I agreed to make a thread storage board for my sister.
It's basically a 24 inch by 24 inch plywood board, 1/2 inch thick, with a grid of holes drilled every 1 3/4 inch from center to center. The holes will start off set from the corner by about .595 so that an even number of them will be centered on the board. I figured I can get 14 holes in the Y direction and 14 holes in the X direction. The holes can be 3/8 inch deep. I'll put a piece of dowel rod into each hole. The spools of thread will go onto the dowel rods.

Now the part that has me stumped is, she wants the holes on a slight angle. I figured all I have to do is prop up one side of the board 2 3/4 inches to the top surface of the board. This will give me an angle when I drill the holes.

What I can't figure out is how to account for the board being on an angle so that my Z moves are correct for the hole depth and it doesn't crash into the high side of the board. I think I just need one row of holes in the Y direction, then just move back to Y=0, move X over 1 3/4 inches, then repeat the row of holes again. This would assume the high side of the board is at Y=24

I have an older PRT96 with ver 3.4.27 software.
I do not have part works.
I've created a file in the drill press tool but it doesn't have a way to compensate the Z depth to account for an angled board.

Any suggestions?

[curtiss]

I think you could run each row one at a time.

0,0 being the start point over the first hole, say z at 1 inch above work.

After the first row, move over the distance to the next row and re-zero.

Run the file again and repeat.

Either that or start the file on the high side, and set each row to a different depth and different toolpath.

[srwtlc]

Mayo, being that your of about the same vintage as myself :) (2000-2001), you may have an old copy of VectorCam lying around. I've done this many times with it by drawing the part as desired on the flat and then rotating it around the x or y axis to the proper angle before toolpathing.

[Mayo]

I do have a copy of Vector 9B but I never could figure out how to use it.
The user interface was less than intuitive and from what I remember, assumes the user has a knowledge of terms that I just did not have.

I guess I'll take the route that Curtis suggested - Zero each horizontal row, then after that row is drilled, move up to the next row and Zero again, etc.

Is this something that would have been easy to do visually in a program like ArtCam or Aspire or some other program?

[Gary Campbell]

Mayo...
setup your material. Toolpath only the first row. Run all rows (including first) using 3D offset.

You can calculate the offsets as follows:
I assume piece is flat in the Y direction and tilted up with the +X end higher than the 0.

Based on this...
Your Y offset would be zero
your X offset would be 1 3/4 (for each row accumulative after the first)

2.75" / 24= .1146" of rise per inch of run
if you zeroed to a flat surface....

1st row would be .595 * .1146 = .0682 for the Z offset
each row after that would add: 1.75 * .1146 = .172 added to Z offset each time you move to next row

1.75 added to X offset each time you add a row
hope this helps

Using the 3D offset will move your Z safe hgt up as each row is cut and negates long plunges for 1st rows

[dana_swift]

Another option is to toolpath one row, then rezero on the top of the material before cutting each row, then as the thickness decreases, it is compensated for by the new ZZero.

If you only have to do this one time, it is just a bit more inconvenient. If you have to do this cut many times, it is probably worth a more automated method.

If I understand you want the cuts to be a consistent depth relative to a sloped surface. If not, ignore this.

Hope that helps-

D

[robtown]

Have you thought about a drill press and a jig?

Sometimes the better answer IS to simply cut that piece on the tablesaw...

[Mayo]

Hey thanks everyone for the suggestions.

I don't have a drill press or I would have considered trying it there, although the boards are 24x24.

I have two boards to make - each having 14 rows of holes.

I now understand the equation for determining the slope of the board - thanks Gary. I don't quite get the procedure for inputting the new Z for each row. After I drill the first row, would I have to put the tool into relative mode, add the .172 Z offset, move X over 1.75 for the next row, then put the tool back into absolute mode, and run the drill file again using 3D offset?

Another question about 3D offset - if the drill file has an X and a Y offset at the beginning of the file, won't the 3D offset ignore this?

Sorry if I'm so dense about this but it's not a way I have used the Shopbot in all the years I've had it. My typical procedure is to create a design in SignLab, automatically generate a toolpath, open the toolpath in the Shopbot software and cut.

[curtiss]

You could use the bot to lightly mark the holes say .05 deep

and then use a hand drill and a simple jig, drilled to the angle you want to drill them the rest of the way...

[gene]

If you drill the holes on an angle then the bottom of the thread spools will not be flat to the board. I would drill then straight and cut an angled strip and attach to the bottom of the board. I did several for my wifes threads and they worked out good. does she want to hang the rack on the wall?

[Mayo]

I got the boards done.
To accomplish it, I first Zero'd Z on the flat, then I ran one row of holes on the lowest side. Then at the end of that file, I did a SR command, moved Z to 0, then moved Z to .172, (the amount the angle increased each row) then moved X 1.75, and then the next file did a SA command and ran the holes. The end of this 2nd file had the same commands to move the Z and the X, and I repeated this with 14 files.

I couldn't get the 3D offset to account for the Z because of the safe Z height and it kept getting me more confused. Every time I tried it (without the Relative moves mentioned above) the Z would never drill the holes - it would always wind up above the board.

The reason I had 14 files rather than one file that I repeated, was because I couldn't figure out how to move the X where it needed to go and Absolute mode vs Relative mode made my confusion even worse. My design software laid out the rows of holes where I wanted them with the exception of not taking into account the slope for the Z, so that's why I decided to use Relative moves in the files for each row, and after about 15 tries on scrap foam, I got it figured out.

I know I could have done them much faster and easier by drilling them flat and just putting a spacer board at the bottom, on back but I was challenging myself to learn a new way of doing something. Usually when I do this, the lessons learned wind up helping me in some other project down the road.

So it took me all day... and it didn't turn out absolutely perfect, but it turned out good enough for what it is. I used scrap plywood I had laying around for two years and it wasn't absolutely flat, so some holes are deeper than others. Plus the way I had it propped up on the angle allowed the board to flex somewhat while being drilled.

One board got grooved in a few places because it was higher in those spots.

It doesn't really matter that the spools won't lay absolutely flat to the board - it's not a show piece - just utilitarian basic storage.

Now my sister gets the job of cutting 392 dowels!

Once again, thanks everyone for offering suggestions.

[Gary Campbell]

Mayo...
I have mispoken in my earlier post. I was explaining the "in the file" method as a way for you to do it from the console with the fill in sheet.

I was assuming that you could enter the x,y and z offsets directly in the fill in sheet. This is not the case. Only proportions can be entered. Even tho proportions could be used, I am not familiar enough with the process to be able to explain it to you.

I can however, give you an explanation of how I do this "in the file" and hopefully it will allow you to accomplish your drilling.

Asssume PWks or VCPro
set home position to .595,0,.5
select 1st row holes and toolpath
Remove header info
save file (example drill_row.sbp)
Make new file with header info, but no moves
write file as follows: (after header)
FP, drill_row.sbp
J3, (.595 + 1.75),0,(.5+.172) (I showed math so you can repeat)
FP, drill_row, 1, 1, 1, 1, 1, -0.00, 0, 0, 1, 1 this moves to second row and runs file in 3D offset )
J3, (.595 + 1.75+ 1.75),0,(.5+.172+.172)
FP, drill_row, 1, 1, 1, 1, 1, -0.00, 0, 0, 1, 1 (3rd row)

add as many lines as needed

[tmerrill]

I know this doesn't help Mayo and he did say he didn't have Partworks, but one option would be to use the Fluting tool in Partworks/VCP/Aspire to "drill" from the back to the front with the material flat on the table.

The backside would be elongated with one side at the angle you have calculated, but the hole on the front would be a clean circle (or close to it) for a good appearance. The dowels would be glued to the angled side and perhaps a small brad or pin inserted to hold it in place until the glue dries. Definitely not the strongest joint, but for thread spools, or something light, it should work fine.


The layout started with one vertical line 0.25" long, then using the Array copy tool you create a 14 X 14 array with the 1.75" spacing. Select them all and use the fluting tool to calculate the toolpaths.

Tim

[ssflyer]

Another thought... I created a rectangle the size of the material, and created a flat shape tilted to -10 degrees ( this could be anything, depending on what angle you set the material on the 'Bot) then simply created the array and toolpathed the holes with "Project toolpath onto 3D model" - I don't see why this wouldn't work with a single toolpath, as long as you knew the angle you had your piece mounted at.