[HuFlungDung]

Originally posted by wms
HU,
snip
I'm sure you already know that these setting are located in the OneCNC file: OneCNC-xp/mill expert/setting/users/default (or any named acount you have set up)

Dammit, WMS, you are wrong again. I didn't know that

Its a good thing to have these discussion boards!!

[wms]

Hu,
I havn't finished that big bucket of crow yet, want I send some up your way? I did get all the egg of my face though.

[wms]

Applicable versions of OneCNC:
OneCNCXp all types

Description of situation or difficulty:
Needed a way to wrap lettering around arc then extrude.
In XP there is "Chain text" funtion to wrap text around an arc. But this funtion vectoizes the text when it applies it to the chain.
So this text is not a surface. So it is not possible to use the extrude font funtion under solids maker button.

The solution was:
1: Use the "chain text" funtion.
2: Then in the surface menu, use the " surface from curves" funtion to surface the individual letters.
3: Then in the solids menu use "Extrude surface" funtion.


(Thanks to Mike Reyes at OneCNC for his help on this problem)

[HuFlungDung]

Keep the articles coming, WMS, we're reading

[wms]

Thanks Hu,
Good to know someone reads these ramblings. Hope you can glean a small amount of info from them.

[wms]

Applicable versions of OneCNC:
Xp vesions

Description of situation or difficulty:
Needed away to machine an island with one or more "keys" around it. This is kind of hard to explain so follow along.(If you want)

The solution was:
A real mind bender
Radial roughing and Radial finishing.
As follows:
I used file mill steep wall machining inch.xfa as a mule file. It's in the sample files at xfa/samples. If you want to try this yourself.

Open up the file and
1) Extract a curve, the top circle. (see photo 1 wire frame)
2) Create a point at arc center. (the aqua one in photo) you need this later for start point.
3) Open up nc manager and start a new tool group. Number #2.
Highlight the new tool group by clicking on it.
4) click on the model toolpath button and select "smt rought"and "z level" .
5) select ramp, 2 degrees, climb mill.
Then select 1 inch mill.
At the cut option box, set minimum for finish to .060 and step over .500 and depth of cut to .075.
At boundary setup box check the extents box and the normal box.
Boundary of toolpath, leave the automatic boxes checked. (it will figure out were it needs to go)
Now wait...... whistle if you want..........while it crunchs numbers.


6) click on the model toolpaths again and select "smt finish" and "radial"
7) select the point you created at the start.(see I told you you would need it. )
8) Now select a 1/2 ball mill.
9) when you get to the "radial option" enter start angle 0 degrees and step 1 and included angle 360. then leave for finish .050 and suface tolerance .0002.
10) At the boundary box: check extents box and normal.
11) boundary of toolpath same as before leave the auto boxes checked. click finished and wait.......whistle some more......crunch, crunch, crunch.

12) click on the model toolpaths again and select "smt finish" and "radial"
13) select the point you created at the start.
14) leave the tool the same as before. (1/2 ball mill.)
15) when you get to the "radial option" enter start angle 0 degrees and step 1 and but now included angle 270. then leave for finish .000 and surface tolerance .0002.
16) At the boundary box: check extents box and normal.
17) boundary of toolpath same as before leave the auto boxes checked. click finished and wait.......whistle some more......crunch, crunch, crunch. better go get somthing to eat....

Now for the fun, select tool group #2 then post, then simulate, leave the stock size auto box checked, (again it will figure it out) set the slider button to about half way between turbo and slow. Click on ok, and eat what ever you went to get.......crunch....heavy math here......

And you should have photo #2.(rendering)

This is only an example of what you can do. Let's say you needed to put 10 keys around you island, You could do that. By radial cut that start and stop at different degrees on your model.

The hard way to do this same thing would be to construct all kinds of different sufaces or solids and merge and cut and merge and cut. Better to do it the Easy way.

[wms]

Sorry photo #1 didn't get attached to the post above. .

So here it is.

[wms]

Here's a tip if you are profilling a chain.

This is a pocket in a part that I needed to run a .050 corner rad mill around. I didn't want to spend the time to finish mill the radius with a ball mill. Onecnc will do that very thing. But sometimes it makes more sense to just use a rad tool.
You can't see all the pocket but it has radius at all corners as most pockets do.

If you look real close( sorry the pics are not better, hard to get lots of info on to screen), at the top picture you will see that the ramp on to the chain (green tool path) is outside the actual toolpath. Here I picked the Red line as the start of the chain.

If you look at the bottom pocket you will see that I broke the line in two, with divide, and picked the Red line there as the start of the chain. The second one is lots better as it ramps out in the pocket as opossed to in the corner. Here there is plenty of room for it make its move with out any interference.

You also can adjust the radius in / out to different setting to help in these situations.

[HuFlungDung]

Good tip, WMS. Sometimes I find it's so easy to miss the simple solution

Thanks for resurrecting this thread, too. It was kind of good to review the contents of the rest of it.

[mlinder]

Hu and WMS,

I think a nice addition to Mill Expert would be the ability for the software to automatically start the chosen pocket/profile at the midpoint of the entity selected for the start of the chain.

I use Mastercam for 2D profiling and this is a check box option which saves huge amounts of time having to do as WMS does-breaking the entity into two pieces (I used to have to do this with Smartcam years ago).

Maybe OneCNC can add this to the "want list"?

Mark Linder
(Alas, I have no cool Avatar yet)

[hardmill]

What do you have in mind M, I'll find you an avatar

PEACE

[HuFlungDung]

Right on Mark. Good to hear from you!

Onecnc tech spport does read here, so I'm sure if there is nothing forbidding this from happening, that it could well show up as another feature.

Only this evening was I playing around with the merge function in Onecnc, when it dawned on me that not only can I merge a CAD drawing, but also, its CAM information comes in with it. Granted, at this stage, the incoming file must have its components located in the proper place, so maybe this does limit what I am imagining doing. But the possibility exists for sort of a library of premachined features.

Maybe other guys knew about this and were hiding it from me.

[mlinder]

Hardmill,

I will definitely give it some thought. Thanks for the offer!

Once I define the persona I would like to convey here, you'll be the first to know.

You would need some kind of jpg, gif, or such for creating it, right?

By the way, being more or less a 2D (Mastercam router) guy who recently bought OneCNC Mill Expert, I have already learned so much useful info on how to use Mill Expert from the contributors to this board.

Hopefully, I can add some useful tips/tricks and offer insight on various relevant subjects.

Mark Linder
(soon to have an avatar!)

[mlinder]

Hardmill,

OK. I have a pic I would like to use for my avatar. It is 150 x 150 pixels, though (needs to be 85 x 85?). I have attached it for you to check out.

Yep, I like to ride quads in the desert. I live in the San Deigo, CA area and miles and miles of dunes are only an hour and a half from my home.

Let me know if you need anything else.

Thanks!

Mark Linder
(Oh, so close to having an avatar, now!)

[cncadmin]

I did it for you.

[hardmill]

Glad to see you found one.
PEACE

[mlinder]

MY LIFE IS NOW COMPLETE!

Thanks a lot you guys.

Mark Linder

[mlinder]

Ummm, I meant San Diego - not San Deigo.

You would think I would get that RIGHT after 44 years. Geez.

Mark

[wms]

OneCnC XP series (may apply to 2000 series)


Here's a little tip if you like me use dwell in your drill cycles. Or any other cycles.

If you enter 300 (no decimal point) in the dwell box. You will get 300. (with a decimal point) in your posted code.

This changes the dwell time from 300 milliseconds to 300 seconds.
That's 5 minutes guys.

But if you put a "space" after the 300 ( no decimal point) then it outputs 300 no decimal point.

Much better

If your control needs the decimal point then you only need to enter the number.




Thanks to James at onecnc au for the tip.

[wms]

Xp and 2000 series.

In an earlier post Hu was asking about verify one or two funtion and how it can sometimes make your scratch your head. I suggested that he use "tape measure".

I have also found that is you go to a normal view, (top, side,front,ect.) you can use the dimension funtions to verify entities that are not on the same plane.

Say you have a line that is at Z zero and a hole location that is at Z -.500. If you select top view and use dimension, horzontal or vertical, (depending on the entites) it will give you the distance in that plane. So you can check things to see if they are where you want them. Then just use the undo to remove the dimesion.

The "tape measure" measures end points so sometimes it's not what you want to check. Between the two you can find about anything you need to know.