CAM setup for raised text

[difalkner]

A friend asked me to make a sign for his medical urgent care business and I'm trying to figure out how to do this quicker.  The medical cross will have a standard medical symbol engraved within the cross boundary but I think I can handle that part.  So how can I set this up such that after cutting all I can with the 1/4" bit I can follow up with the 1/8" bit for the areas the 1/4" bit can't get to without having to cut the entire toolpath with the 1/8" bit? I've read some software, such as Vectric, has a setting by which you can have the smaller bit only cut what the larger bit can't get to and that's what I'm looking for in Fusion 360.

One thing I can do is choose the inside of the letters like 'o' and 'e' to have the 1/8" bit cut just those but that doesn't help on the inside of the other letters which won't be clean and sharp with the 1/4" bit. I can change to plunge instead of helix and get to most of the text with the 1/4" bit but it still won't get to all the pockets or be as sharp.

Here's the Screencast link - http://autode.sk/2hxl16L

Thanks!

David

[Steinwerks]

I would recommend switching to 3D Pocket and utilizing Rest Machining. For the first toolpath From Stock will work great, and for the second with the smaller tool make it From Previous Operations.

[difalkner]

WOW!  That was so easy but I never knew to do that.  Thank you so much! 

In my sample I forgot to add the engraved text thinking it would just skip right over that but apparently it's just big enough that the 1/8" bit will fit so Fusion 360 tries to accommodate by milling where it can.  The only thing is that I want to handle that with a 60° V bit.  How do I make the second 3D pocket toolpath with the 1/8" bit skip over the engraved text? I tried putting the engraving step right after the 3D pocket clearing with the 1/4" bit and the simulation looks good but when I add the second 3D pocket clearing with the 1/8" bit it still wants to hit the engraved letters.

[Steinwerks · Accepted solution]

You can limit the toolpath by calling the surface you want to stop milling at the bottom of the toolpath on the Heights tab and selecting the Flat Area Detection checkbox in the Passes tab. Then you can use a 2D Engrave toolpath for the letters that will do the v-carve style engraving I expect you'd prefer.  That's what I'd do, anyway. Good luck!

Edit: here's a great video on Engrave by Lars Christensen:

[difalkner]

WOW again!  I'd be dangerous if I knew anything - LOL!  It's so easy when you do it right, it seems.  That did it for me, at least on the simulation.  I'll try the sign tomorrow if I can get some free time.  I watched Lars' video quite a while back when I knew even less than I know now so maybe watching it again will be a good thing. 

Thanks again!

David

[Steinwerks]

No problem! Let us know how it goes!

[difalkner]

So I'm back on this sign for a friend and after a few changes am ready to cut it... but I can't get it right - ugh!  I've attached a couple of images and can give access to the file if needed (though I'm not certain how best to do that).  I didn't try to draw the exact perimeter in Fusion 360; just went with a circle about the same overall size and figured the little bit of air cutting won't amount to much wasted time.

The sign is about a 24" sort of circle ranging from about 3" thick to 4" thick and is a slice from a Pecan tree.  This is a piece of one tree cut down to build the new facility and thus has some sentimental value (i.e., it's the only one I have so I need to get it right the first time).

The images are of the actual Pecan slice with the intended letters and symbol overlaid to scale or at least close.  I don't have to make the slice a constant thickness so all I have to do is place the top plane level to my CNC table and face it so my plan is to do that with 2D face and a 1.5" flat bottom bit, same one I use to level my spoilboard.  My intention was to then use the same 1.5" bit to hog away everything it can around the letters and symbol just to cut machining time to a minimum.  However, when I try to set that up in 3D parallel that bit isn't available to me.  So the largest bit I have that shows up in that profile is a 1/2" flat bottom end mill or router bit.

In my CAM setup I have tried 2D and 3D pocket, 3D pocket, 3D horizontal, and all work to some extent but none work to completion.  Some don't have rest machining to continue from previous operations so the subsequent operations with a smaller bit just takes forever and it will be cutting air most of the time.  Some seem to have a lot of collisions regardless of how I changed the settings.

My CNC router is a Saturn Pro 2x4 stress relieved welded steel frame from Fine Line Automation and I designed, sourced, and built everything else.  It has a 3Kw water cooled spindle with four 637 oz. in. NEMA 34 motors and I'm running Mach4.  I have rapids limited to 750 ipm but it will go much faster.  It's a stout machine and as it sits is about 600 lbs.  This is my first CNC so I have a lot to learn but am getting up to speed best I can.  I offer these specs more to say that it should cut this Pecan slice with no problem except that I can't figure out how to do it within Fusion 360.

So I am at a loss on this... what's my best approach going to be besides carving this by hand?  And I REALLY don't want to do this by hand... LOL!

Thanks, guys and gals!

David

[daniel_lyall]

Curtis did a vid on doing inverted text here https://www.youtube.com/watch?v=k2AsvN7ofcU some ideas in there that help a bit

[difalkner]

I definitely learned some things in that video by Curtis and also watched one by Winston (I also need to make a branding iron!).  But Curtis' video only showed me how to clean up the points in letters like 'A' by using engraving. 

What I need most is how to level everything around the letters and symbol - 3D parallel, 2D or 3D pocket, 2D or 3D contour, etc. - and then switch to smaller bits to get the detail in the letters and symbol without having to recut everything with the smaller bits.

For instance, I can use a 1/2" end mill on 3D parallel and set the depth of cut to 0.125" each pass and the machining time is about 90 minutes.  I can copy that profile and switch to a 1/4" bit and it cleans up what the 1/2" can't get to and that machining time is about 6 minutes.  When I try to set it up with a 1/8" bit for the final cut it won't generate a toolpath or it only cuts one small place and is over in seconds.  Now, I don't know if parallel is the proper profile to use but it gets me close to my final goal.

One thing I have done is use 3D horizontal with 1.5" bit, then 3D parallel with 1/2" bit followed by 1/4" bit, then switch to 2D contour to clean up the letters and symbol although the simulation looks like it may not be just right on the symbol.  But this gets me pretty close and maybe that's the best I can do - fair number of tool changes and a little over an hour machining time.

Ancillary question - with all of the tool changes my assumption is that I set zero on the same place on the work piece each time so that they all cut the same depth.  Is that correct?  I don't have a Z touch plate yet.

Ideas, comments, do I need to upload or share the file, etc.?

Thanks!

David

[daniel_lyall]

Yep post your file, It's just to check for any problems And show you on your file, It's 100% easier than haveing to make a guess.

The tool height setter that's a easy one, depending if your controller is active low or high I cant rember what you used.

All you need is a bit of a metal wired into an input and set your probe pin to that in the controller plugin and M4 on the probe setting in inputs, depending on if you controllers is active high or low you ground it out through the spindle or a ground wire connected to your -common to the tool. or you use some type of switch.

I just 3D printed a tool height sensor and hot snoted a momentary switch into it it's just a copy of one I saw on cnczone.

There is a offset setting where you put the object's height in then when you touch it the machine know's where the work Zero is.

Setting it to start with there is 2 options, top of your bed and cutting is a + or top of the work then all cutting is -, if you will lose where you set the zero in the first op use the bed.

to save your file and post it

Go to File -> Export and save as a .F3D Archive File and attach it to your next post

[difalkner]

Much appreciated, Daniel!  Yes, I need to make a zero touch plate.  Eyeballing it and using a piece of paper just isn't quite good enough - LOL!

I am attaching the file along with a screenshot of the four operations that seem to work or at least gets me close to the final piece as desired.  I just don't know if this is the best and most efficient way to do this little job.  Because I want to learn more about the entire process of CAD to CAM to CNC I keep searching for better ways and I hate to lock onto this four profile process if there's a better way and I'm just missing it.

Thanks again!

David

[daniel_lyall]

I am working on your file now, One thing I was told about routing wood, think of it how stainless steel gets machined, get the heat out as fast as you can other wise you get work hardening, In a router it will be fire.

What just boils down to take a good size chip out at a decent speed, you machine is rigid enough for you to go fast and to take a big chip the only limit you have is Hp.

So you can do most ruff cutting at 50% depth of cut 50% width of cut up to a 1/4 inch cutter you may be able to go deeper and wider, that's something for you to test on a bit of scrap wood.

So far I have done A faces cut to clean the top of, A 3D adaptive with a 1/2 inch cutter, then a another 3D adaptive with a 1/4 inch cutter these 3 will clean 90% of the wood out.

Then a profile around the letters and symbol useing a 1/8 cutter.

then the rest will be up to you, you can now just do the finishing cuts or a Vcarve whatever you like all the hard work is done.

You will see in the toolpaths what I have it set to, It's less than what I would do with my big one but I have found the limits of it, once you find your machine's limits depending on the wood you can do bigger or smaller depth and width of cuts.

[daniel_lyall · Accepted solution]

@difalkner Here is your file back I have given you 2 options the first one is a conserved toolpath the 2nd one is a bit more aggressive, you may need to change the depth of cut on the second toolpath.

If you have a look at the first set of toolpaths, if you don't change anything hit cancel if you do hit ok they take quite a bit of time to generate. 

[difalkner]

Hi Daniel,

Sorry it took so long to respond but your solution worked perfectly!  I combined the two profiles you prepared, changed the feed rates, but that was just specific to what I was cutting and my machine capabilities.  The reason I took so long to respond is that I wanted to cut the slice of Pecan tree so I could post photos and it was a while before I could get to this to cut but it is complete and soon to be mounted in the office.

Thanks so much!!

David