Need Help!- Programming a Router to cut a "sine wave" in hardwood?

[ZeroStar]

Hey guys. Been working with our company's CNC for about a year now. Never had any formal instruction, just learned G-code by reading, so there are some gaps in my knowledge.

Until now, I've only had to cut things which would be considered 2D jobs, but now my boss has asked me to create a hardwood die on our router. Basically he wants me to carve the surface up to look like a piece of corrugated metal.

The boss's thought was to go back and forth with a lot of straight lines incrementally lowering them as we moved across the sheet, but our test cut for that looked horrible. I'm really hoping there is a way to code it to cut a bunch of side by side waves so that the curves are much smoother.

Is this possible? I know there are g-codes to make a circle on the X-Y axis, but I haven't seen any Z-axis codes other than go up or go down.

Help please!

[JWK42]

How far from crest to crest? Are your waves perfect radii from top of crown to the pitch diameter or mid point of the wave. You could use a ball end mill to cut the valleys and a corner rounding end mill to cut the crests. Each crest would require a pass down both sides.
You could also cut it with a series of side by side radius cuts across the crests and through the valleys using a ball end mill and stepping over between each pass as you suggested.
What kind of a control is it? Do you mave macro's?
If you can describe your pattern a little better I'll bet someone on here can help you

You can change from your standard interpolation mode
G17 ( X-Y Code ) G02 or G03 rotates around Z Axis
to this
G18 ( X-Z Code ) G02 or G03 rotates around Y axis
or this
G19 (Y -Z Code ) G02 or G03 rotates around X axis

to make the sine wave across the crests and valleys

[HuFlungDung]

You may be able to command circles in other planes by switching the plane with G17, G18 or G19. Depends on what the controller allows, I guess.

I'm not certain that having the tool bobbing up and down is the way to go about this sort of surface. I would think that parallel passes along the corrugations would be more productive. That way, you only need to generate a few start points along the curve at the beginning and the end of the sheet.

[ZeroStar]

Apologies in advance for my lack of knowledge when it comes to the correct terminology for things. What we're trying to do exactly is make 2 identical plates that can be mated together. The exact wave pattern isn't decided on yet (sorta depends on whether this can be done or not) but ideally both the trough and the peak would be 1" radius circles so that they will mate with the other piece. I was looking at the ball router idea earlier, but the cost was a bit out of our range, since this is still an exploratory project, and since we normally only cut 2D stuff out of plastic, all I really have to work with are 1/4" and 1/8" bits.

Is there a way I can upload a pdf or something of what I'm trying to do?

Thanks again for any assistance.

[HuFlungDung]

When you make up your post, select 'Go advanced' then you will get to a page where you can manage attachments, and then you can add pictures, etc.

[ZeroStar]

Ok, here is a side view of a section of what we want to do.

Think this, but on a larger (4'x8' sheets) scale.

[JWK42]

Ok!!
I'm trying to wrap my head around this job. If you are making this sine wave pattern in a 4' x 8' sheet, that is a lot of material to remove with a .25 dia tool. You will be 2.0 in. deep from crest to valley. That's a lot of cuts and a lot of tool sticking out of the collet. I'm not very sure you can do this job with a .25 dia cutter sticking out 2.0 in.
You could make your roughing cuts with a series of straight cuts,as you said earlier, remove most of the material. Then do the cuts across the crests & valleys using G19 and G02 & G03.
Do you have access to a CAD system that write your code for you. If not you need to let us know what kind of control and if you have macro (variable) programming. This would be a really long program to do long hand.

[ZeroStar]

We've got BobCAD, which makes really messy, incomplete code by my experience, and no one here knows how to do 3D modelling anyway, so the best I can do is trying to transpose 2D stuff.

We've got a Practical CNC machine with WINCNC controller (I think). No clue about the macro thing. How would I check?

[BobWarfield]

This is going to be painful to do well, but here are some thoughts:

First, I would skip sine waves because the shape of the wave doesn't matter so long as it mates.

Second, can you live with any shape that mates, or must it be a smooth curve? It'd be easier to machine grooves with square corners that mate, for example.

Let's assume it has to be curves. Let's further assume you can't do anything crazy on the cutter front. You really need ballnosed cutters to do it right. It's a 3D profiling job. You write a pass that cuts the curve using the Z to raise and lower, you stepover some amount that is less than the diameter of the cutter, and make another pass.

BTW, Excel is really handy to create such g-code programs. Use the number formulas to calculate your Z heights and then use string formulas to create the g-code. Cut and paste into your g-code editor.

If you don't have a ballnose, your curves will be slightly off at the bottom, but that may not matter as this doesn't seem a precision job. Just use a smallish cutter diameter.

The less you stepover between passes, the smoother the curve will be.

If your g-code uses line segments instead of arcs, the shorter the segments, the smoother the curve will be. You can again use Excel to generate those segments.

Last thought: this job will run slow! Hope you don't need to make 1000 of them. If you do, you're better off having a cutter that is shaped to do the crest on either side and the value in the middle. Then you just do one pass down each valley and you are done. I'm sure there must be a router cutter like that, but no idea what it costs.

Cheers,

BW

[JWK42]

Goto MDI mode and type in #100=2
hit cycle start and see if you get an error message about unknown code.
I have checked with Google and can't find any examples of WINCNC code.
The #100 series is Fanuc based
If you have any examples of code from the control look for "#" or "E1=" or "IF[" or "GOTO" or "SIN" or "COS" or "TAN" these are codes that would indicate variable programming.

[Andre' B]

It has some kind of macro language.
http://www.wincnc.net/feat_macro_languages.php

But it does not seem to be anything like Fanuc's macro-B.
http://www.wincnc.net/webfiles/CNC%2.../WinManual.pdf

Edit:
And if you are going to form a sheet of some kind between these dies you need to make room for the material. The radius on the crest needs to be smaller then the radius in the valley.

[glenthemann]

dont know if youre controller supports it, but the ones I have used have the SIN function.

Youd need to use a macro, and have it work something basically like this
P1= x start position
P2= x end position

WHILE P1 <= P2

G0x[P1]y0.0z[SIN[P1]]
G1y-5.0 (however long you want the ridges to be)
P1=P1+0.001 (the value here depends on how perfect you want it to be obviously)
G0y0.0z0.05 (z value here is also up to you, its the tool retract)

WEND

this will loop until P1 is greater than P2, and the Z values are found by finding the sine of your current x value.

Of course youd have to put in considerations for comp, etc, but its just a basic idea of how I know I would approach it. You can manipulate the sin to compress, or expand the wave form.. im sure if you remember a little high school math it shoudlnt be an issue for you to get the proper peaks and everything you want.


Keep in mind I am a complete noob to CNC programming, but I have done a lot of other programming in the past that CNC Macro programming is a lot closer to, so yeah, Goodluck

edit::

oh and I guess I should mention that youre going to have to do more math because with a round cutter, the cutting point is not going to be similar each time and you want the ball of the cutter perpendicular to your surface so its actually not quite as easy as saying go over this amount and this depth each time..

youd really be best off with some sort of cad software to profile it out for you