Generating code for bed levelling

[lifeaquatic]

Hi there,
I need to level my MDF bed, but I cannot find any obvious machining paths/templates to do this. Do I just use the pocket function?
Many thanks

[EddyCurrent]

I think most people use this method;

1. Draw a polyline to represent the Y axis length of the MDF bed
2. Use a Profile machining operation with the "Cut Width" parameter equal to the MDF bed X axis length.
3. Set parameter "Milling Direction" to "Mixed" to speed things up.


Of course you can swap the X and Y above if required.

[pixelmaker]

When I level, I never use mixed toolpaths. This speeds up the work, but with different milling directions I get minimally different heights through the face mill.

ralf

[Dragonfly]

I don't think this is an issue on a MDF board.

[Dragonfly]

Sometimes I use an MDF board over the Alu table and here is how I level the surface at 45 degrees strokes. Using Pocket and Transformation matrix both on the geometry and the MOP. The first is tilted 45*, the latter @ -45*. I think David was the one who taught me this trick.

[lifeaquatic]

thats great, thank you all for your help! I'll give the first method a try today

Cheers

[chuckeroo]

I gotta ask why not use a pocketing MOP? Perplexed.

[Chip Owner]

I gotta ask why not use a pocketing MOP? Perplexed.

Seemed the obvious way to me also, so that's what I use.

[lloydsp]

Ralf wrote: "...but with different milling directions I get minimally different heights through the face mill."
-------------
Ralf, I bit my tongue when you wrote that, but I just cannot hold it in!

If you get slightly 'dished' cuts, you'll get them in any direction you cut.  They're happening because something is loose in what is holding the spindle perpendicular to the work surface.  It could be in the spindle mount.  It could be in the gantry bearings.  It could even be due to 'play' in the spindle, itself.

Were I you, I'd be working on the rigidity of that setup.  The symptom says you've got something to fix!

Lloyd

[Bubba]

Ralf wrote: "...but with different milling directions I get minimally different heights through the face mill."

Agree with LLoyd, but it also could be the spindle need to be trammed in to the table surface..

[lloydsp]

Bubba wrote: "...but it also could be the spindle need to be trammed in to the table surface."
-------------
Yep.  Thanks for reminding me!
Lloyd

[pixelmaker]

Hello Loyd
no, it is certainly not due to a loose spindle.

One of the very basic principles of face milling is that the cutting forces are always uniform during face milling. When the milling direction changes, as shown in Eddy's example, the cutter stops. Both the stop on the material surface, nor the move out of the material and back in, to have the stop outside the material, is according to the textbook of face milling.
If I stop on the material, the milling is minimally deeper at this point, if I move over the edge of the plate to set the stop outside the material, the cutting forces change when moving out, and when moving in, the increasing cutting forces can cause vibrations.
The cutter must always be constantly engaged.


Another thing that speaks against the changing tool paths is my base plate made of PMMA because I mostly cut PMMA . In principle, face milling should always be performed in constant force. In the area of an overlap, there is different heat in the pmma where the cut is made than in the overlapping area. As a result, a touch more is always cut away. With alternating tool paths, this area is in the middle of two tool paths. This must not be the case either.

I know it depends on the mill or the material. A wobbly router may have problems with the spindle wobbling. But then the mill also does not manage to stop the cutter. If I'm milling an MDF or wood, none of that matters. But if I'm milling aluminum or PMMA and want to achieve a really smooth surface, you shouldn't alternate toolpaths.
When I mill cast PMMA blocks, I see the difference in how much I have to grind before polishing.

ralf

[lloydsp]

Well, Ralf,
I understand your situation well.  I work a little with Plexiglas (PMMA), but most of my parts for clients are done in 'foamed' vinyl (also rigid, in the form in which I purchase it).

I was just 'interjecting'.  If you're happy with the results you get, then that's all that really matters -- yes?

Lloyd

[Dragonfly]

@ pixelmaker
I work predominantly with Aluminum (most often 6--- alloys). Have tried different approaches, step over values, etc. to produce as smooth as possible surface. Your post confirms some of my personal conclusions. There's  one thing more which I think also affects surface marks - no matter what general cutting direction is selected the cutting edges always do both conventional and climb with regard to the surface.

And because usually one starts with a square or rectangular piece of stock I am really missing a feature in CamBam to do pockets on regular geometric shapes with a tool path that is a constantly expanding spiral, i.e. avoiding the 90* sharp side moves and thus maintaining cutting force constant as much as possible.

[pixelmaker]

avoiding the 90* sharp side moves and thus maintaining cutting force constant as much as possible.

One possibility is to set a constant velocity in the controller.
Then a radius is inserted at the corners which allows to drive the corner without loss of speed.
I use the spiral and the engraving MOP as another possibility. There are milling, e.g. when milling concave hollows, I have divided the spiral so that I can use different speeds. In this way, I can increase the feed rate as the radius increases.

You can cut a spiral with a rectangle and connect the open ends. But I only do the extra work with the file if there is a large number of copies behind it.

I am really missing a feature in CamBam to do pockets on regular geometric shapes

Spiral Pocket +1

ralf