Cutting tips and numbers for 23/32 Plywood

[Lemanskis]

Im trying to cut a 4' x 8' piece of 23/32 cabinet grade plywood into strips about 3.4" wide. When I begin to cut the plywood the router head traces the profile line fine, however once it reaches the end of the cut line rather than plunging deeper and re-tracing the line back, the cutting bit returns to safe height and jogs back to the start of the line. Once returning, the bit plunges deeper into the material and continues the process over.
This would not usually be that big of a deal, but when I need to cut over 500 strips, every minute of CNC time is crucial.

My current tools/settings are:

1/4" downcut bit
16,000 RPM
cut speed 3.0
plunge depth .35 to make 2 passes to get to .7 before final cut
to take care of onion skin.

2 questions:

Is there a way to go back and fourth along the line rather than reset back to the beginning of the line?

Is there anyway to make up time by changing my cutting speeds?

[tlempicke]

You could probably edit the cut file so that the jog back to the start was eliminated. A quick and easy thing you could do to save time is to up the jog speed as much as possible and lower the safe Z as much as you can. I think that what the software is "thinking" is a return to the start point and now do the same thing over only a certain number of thousandths lower.

[kevin]

I dont mean to be a smart ass .How come you dont use a table saw

I,am pro shop bot but I dont think you could beat a table saw in this case

your going to burn out a few bits

[Brady Watson]

Im trying to cut a 4' x 8' piece of 23/32 cabinet grade plywood into strips about 3.4" wide....

Is there a way to go back and fourth along the line rather than reset back to the beginning of the line?

Yes...but it takes a little node editing. You want to alternate the start points on each line so that the green start point is staggered. So line 1 would start at the left side, line 2 at the right side, line 3 at the left side & so on.

Then, make a toolpath for each stepdown you want by selecting everything, and then make a toolpath with let's say a .25" stepdown. Then make another with a .5 SD. Then a 3rd for the final or whatever depth you want.

Cutting strips can be a real challenge when it comes to keeping the material held down. A table saw is a much more efficient way to do this...

-B

[gc3]

I dont mean to be a smart ass .How come you dont use a table saw

I,am pro shop bot but I dont think you could beat a table saw in this case

your going to burn out a few bits

this forum needs a "like " button!

[tmerrill]

Steven,

In the event there is a reason you want to do this on your ShopBot, and you are using Partworks/V-Carve Pro/Aspire, there is a trick that will do what you want, with a trade-off.

Instead of drawing a line, create a rectangle the length you want but with a width of 0.001". You only need to create one, then use the Array Copy tool to create the remaining one.

Select them and set up a Profile-On toolpath with the selected bit. Select Spiral Ramps under the Ramp tab and calculate. This will create the back and forth saw motion you are describing. The number of passes will be determined by the Pass Depth you have set for the tool.

The trade-off is the Spiral Ramp always requires an extra pass to remove the last amount of material. So, as an example, instead of 3 passes at 0
.25" each with rapids in between, you would get a continuous toolpath of 4 passes at the Plunge rate you have set for the tool..

Tim

[Lemanskis]

Thanks for the tips,

I did leave out some (what I thought to be) useless information… Im a student at Wentworth Institute of Technology in Boston MA and this is a class project for 14 of us to complete. It is an Installation project scheduled to be done Dec. 9th and remain up through April. Most people in the class have never used table saws and miter saws before. Right now a few others and myself are dedicated shop people, with the addition of a few others. The less people have to actually handle material the better, and better for me not having to watch over shoulders for hours at a time. Whats nice about the CNC… I can set it up and leave the room, someone else who has little to no training with power tools could watch over the machine while I can work on another portion

As far as getting a table saw we have one but its set up for a dato cut … each one of these pieces needs to be datoed ¾” wide and 3/8” deep down the center to accept a ¾” pipe.
Also each piece has a special profile halfway up the board, and counter sunk screw locations. I guess the milling could be cut first then move over to the table saw to finish the straight cuts.
We are afraid of the precision not being there if we use the table saw. At first it may be but once we get to the 100th cut… 14 sheets later, there are bound to be mistakes.
And we need to cut 500+ (closer to 750 actually) so the chances for mistakes are even greater.

Anyway long story short, milling may take longer but once its set up we can work on other things that need to get done.

Thanks again for the advice everyone.

[Lemanskis]

What do my numbers look like,

16,000 rpm
.35 depth
3.0 feed rate

my rpm seems a little high compared to others (other people cutting wood)
im getting very small chips but mostly dust when one of these sheets is done milling.

Could, or should the feed rate increase because of the high RPM?
or is it maxed out because of the small size of the router bit.

[zeykr]

You don't say if you're using a spindle or router, a std or alpha machine.

For a spindle on an alpha I'd say the RPM is too high and feed may be able to increase some. Post some specifics on your machine and someone can probably make suggestions.

[knight_toolworks]

the problem is that when you cutting one direction it is a climb cut and cutting the next piece in the opposite direction it would be a regular cut. so the parts are really going to vary in width.