Facing, schmacing...just not getting it!

[HankMcSpank]

Apologies, this post perhaps is more to do with general CNC operating (as opposed to Mastercam), but I'm dabbling with the demo as this section seems to have a decent audience. (nods...please feel free to move to a more appropriate forum if you see fit)

My problem - I must have spent the guts of 3-4 hours tinkering to get the most impossibly simple cut simulated properly!

Imagine a rectangle...looking at it in plan view, I want to cut a slot about 6mm wide/deep(approx 0.25") wide into this...no matter which option I use, I cant' seem to get a nice clean slot cut!

I've attached a screen shot ...the slot area I'd like to see are those two parallel green upright lines underneath all those blue zig zagging toolpaths!

What's going on there? (the toolpath is *way* overshooting the green lines!)

Perhaps it's my interpretation of what the toolpath 'action' does?

is this right....

Facing = shave some material off the surface of your material?

pocketing = mill a recessed pocket into your material

I've tried both with varying degrees of success!

What should be my approach to get a nice, clean slot into that rectangular block?

[Superman]

Originally Posted by HankMcSpank Facing = shave some material off the surface of your material? pocketing = mill a recessed pocket into your material I've tried both with varying degrees of success! What should be my approach to get a nice, clean slot into that rectangular block?

2D_Contour
pick the 1st contour R/H side line near the front, 2nd -L/H line near the back
and go from there, set comp ON ( computer, control or wear )( use 5mm tool )

or create a line down the middle, select that and have comp. OFF , using a 6mm tool, no arc on the lead in/out ( but extend the start and finish points by 5mm ) ( tangent )

Facing is just that, it will get rid of all material inside the shape you pick, the rounding on the ends of the path is hi-speed change of direction ( machining is smoother, you can make sharp if you wish

Pocketing probably is the wrong choice for a narrow slot

[HankMcSpank]

Originally Posted by Superman 2D_Contour pick the 1st contour R/H side line near the front, 2nd -L/H line near the back and go from there, set comp ON ( computer, control or wear )( use 5mm tool ) or create a line down the middle, select that and have comp. OFF , using a 6mm tool, no arc on the lead in/out ( but extend the start and finish points by 5mm ) ( tangent )

Thanks for the quick response...with your first option, isn't there a risk that there'll be a tiny amount of wood (MDF) at the small horizontal small lines at the front & the back of my slot? But perhaps more significantly, won't there be curves in each of the inner rectangle corners? (edit: just seen your suggestion to use a 5mm tool - alas, I only have a 3mm at the moment!)

Re your second option,well, as mentioned I don't have access to anything other than a 3mm tool at the moment, so I'd need to think about a couple of cuts....the problem here, is that when I knock up the design in CAD...I put it together how I want it to look - but it's rapidly becoming apparent, for the cutting aspect, my cad design should more represent how it should cut. So for example, whereas my jpg above shows a rectangular groove sitting in the main stock of material, perhaps it should show a rectangular groove going past the top & bottom boundary line - alas, very soon, I'll end up with a CAM drawing that looks nothing like the CAD drawing? Or am I approaching this all wrong?

I'm new to all things CNC & must confess to being slightly perplexed that something as simple as cutting a rectngular slot out of a bit of wood, should be so troublesome (to me at least!)

I'm still not grasping why when I choose 'face' as the milling toolpath option, why the toolpath blue lines zig zag way past over the lines that I selected when setting up the chaining aspect?

[Derek Goodwin]

The facing toolpath is overshooting the lines because it is designed to cut the top surface of a part. As Superman stated, 2D contour is the way to go, it will not leave scallops because the toolpath direction will be up and down on your sample, not zigzagging from side to side.

Here is a 2D contour Tutorial

[Superman]

I'm still not grasping why when I choose 'face' as the milling toolpath option, why the toolpath blue lines zig zag way past over the lines that I selected when setting up the chaining aspect?

Facing
Whether you select nothing (no chains [Mcam takes the defined stock size] ) or a rectangle or any othe shape, mastercam will "face" or clear that feature to a set level, you can alter the "direction" the tool will travel to clear this feature, pitching across at 90° to that direction of travel
eg take a 200 x 50 rectangle angled at 45°, if you leave set at 0° passes the tool will travel parallel to the X-axis, but alter the passes to 45°, and those passes become more efficient.
NOTE!! try altering the angle passes to 90°, 135°, 225°, 315° and see the change

Pocketing
Using the same geometry, Mastercam will keep the tool inside the selected shape, and do "stepovers" to get rid of material, if it is large shape then pocketing this shape is done better with a larger tool, if you were to do a slot where the ends are open, you would modify the pocket ends by a minimum of the tool radius plus whatever finishing allowance (XY offset) you have programmed.

eg 200 x100 block, 20mm wide slot, 12mm cutter, 1mm left on the walls for finishing. Using this info the pocket dims should be extended by the ( tool radius + finishing allowance ) on each end
then
200+(12/2+1.0)+(12/2+1.0) x 20mm wide
= 214mm x 20mm ( this would be the minimum adjustment required )

Contouring
You select can select 1 or more (entities or chains or a combination )
you can have mastercam control how you want the tool kept relative to this geometry selection ( you should play with this feature to understand it's full functionality)
-multipasses- have mastercam do extra offset passes at each Z-level
-cut depths- breaks the distance between "start depth" and "depth" into many Z-level passes
-lead in/out- have the tool descend and retract in a position away from the part features, and also extend or shorten the endpoints of your selected entities before a toolpath is applied.

--these last 3 can all work in conjunction with each other
ie lead in/outs on each multipass toolpath at each depth of cut

to wrap it up, to do your 6mm wide slot using a 3mm tool,
use 2D_contour
multipasses ON ( 2 roughing @ 1.5mm, 0 finishing)
depths ON ( roughing 2mm, finishing 0 )
lead in /out ON ( tangent, line 1mm, arc 1mm 45° for both. extend ON 4mm, use Right pointing arrow to copy LH data to R-side for both sections )

[HankMcSpank]

Wow...Superman - thanks what a super reply. ("You'll believe a man can fly" .....around all the CAM options!)

As it goes I had dabbled with just about all those options, but as a noob, I haven't quite perfected interpreting how to use the tools at my disposal to do the cutting. For example, I had seen while general dabbling that that using multipass starts some way from the actual desired cut line & then approaches it by a set amount each time...but I never made the connection as to how that could help me here cut a slot.

It just goes to show that without the depth of experience, what an uphill task learning how to 'operate' a CNC machine will be ...as a hobbyist, I've spent way too many hours building my machine & I've come to a fairly abrupt halt as I grapple with all the concepts of actually using a CNC mill!

I must be getting a little slow omn the uptake in my mid life years - I'm still not getting that facing bit - you said "Whether you select nothing (no chains [Mcam takes the defined stock size] ) or a rectangle or any othe shape, mastercam will "face" or clear that feature to a set level," ...what's the point of having a facing option, if it's going to go outside the defined shape/feature limits? (that said, I'll have a dabble as per your post later tonight)


re the sample video posted earlier in the thread ( http://www.eapprentice.net/samplevideos/vid53/vid53.htm ) - has anyone taken out an eapprentice subscription & can comment? I'm quite tempted to go for it.

[Superman]

Originally Posted by HankMcSpank I must be getting a little slow omn the uptake in my mid life years .

Bloody hell, I'm the same age as you

BTW. have you 1st looked at the samples that come with the installation.
an example is given for the common features. They are broken up into directories depending upon the strategies used. It would be the 1st point of call, if you are self-learning

Just to rub it in as to how much there is to learn, have a look at the multi-axis section. Then you can say WTF

[cadcam]

put radii at the end as being drawn as a true slot and use "Toolpaths" "Circle Paths" "Slot Mill".

PS did you look at the last posting you did and my reply link: http://www.cnczone.com/forums/showthread.php?t=81477

[cob]

http://www.eapprentice.net/samplevideos/vid53/vid53.htm ) - has anyone taken out an eapprentice subscription & can comment? I'm quite tempted to go for it.


A buddy of mine did subscribe to the subscription and I must say it is perfect for those that are starting out with mastercam it starts from basic to 3d. I say try it . its cheap

[ObrienDave]

The hardest thing to learn is, how to make MasterCam, or any other cam system, do what YOU want it to do.
Not to flame anyone, but, if you ask 50 different programmers, you will get 50 different ways to do the same project.
The point being, there are many different ways to accomplish the same task.
Each programmer has their favorite methods.
It would also be impossible for a software company to have a limited number of cutting methods to address all the different ways that an engineer, and I have seen some real winners, can design a part.
That is one reason why cam software has many different kinds of cutting methods.
Having personal experience with (SHUDDER!) MasterCam 386, I can tell you that some of the toolpath routines are simply there for backward compatability with older Mcam files.
Not to imply that they not useful or that they do not work.
Enough of the rant.

Imagine, if you will, that you want to machine a thick walled shoe box from raw stock.
You could use FACING to machine the top of the box.
A POCKET routine for the inside of the box.
Then 2-D CONTOUR the outside of the box.

[cadcam]

Having personal experience with (SHUDDER!) MasterCam 386, I can tell you that alot of the toolpath routines are simply there for backward compatability with older Mcam files.

Not sure what you are saying here. are we talking about certain paths like 2dswept or rulled?

[ObrienDave]

Oops, I should have said "some", not "alot".
Darn, 122 helpful posts, and I mess up one, and the Mods want to question my sanity.
Just kidding.