[HuFlungDung]

Applicable versions of OneCNC:


Description of situation or difficulty:


The solution was:

[HuFlungDung]

There are always ways of doing things that are pretty much undocumented. In my case, the solution is often embarassingly simple, but I still had to make that phone call in to support

So, just quote the above form and fill it in with what you learned. Try to keep it simple, one "revelation" per post, but post as many discoveries as you like.

Applicable versions of OneCNC:
One2000 Mill, likely OnecncXP

Description of situation or difficulty:
Trying to create minimum toolpaths for a near net shape workstock.
Even in a near net shape situation, I always like to rough cut, just in case there is a heavy stock zone, then finish cut.

I know I get stuck in certain modes of thinking and I always think, I've got to use the rough pathing before I use finishing pathing. Not so.

In this case, using Onecnc's roughing paths gave me more toolpath than I needed, or none at all, depending on whether I picked the roughstock boundary or the part boundary.

The solution was:
Use the finishing paths routines instead. You can still offset to leave another pass for a second cut later. In essence, you will get two finishing toolpaths, but you can always rename the first one in OnecncXP's NC manager.

Lesson: The finish routines give you a "net shape" toolpath with no extra stuff to clean out of an extents box, which is what roughing is designed to do.

[HuFlungDung]

Applicable versions of OneCNC:
Mill2000, likely OnecncXP

Description of situation or difficulty:
milling everything down to a certain level and no farther

The solution was:
This one isn't fresh in my mind, but here goes: at first, I was trying to use custom cuts. Custom cuts is necessary if you want to save time and machine exactly to a given plane, such as may exist in the part. Particularly in roughing, you need to make use of custom cuts to ensure that you don't leave a heavy stock above a certain plateau that may exist between your depth of cut options.

But custom cuts does not limit the downward toolpath creation. In this one situation, I needed to go back in and just alter the upward cusps of a mold project. What you need to do in this situation is sketch out a rectangular plane and surface it. Translate it right into your model to the level that you want to cut down to. I'm a bit hazy from here on, but I think you select your model to create toolpaths as per usual, and then select this planar surface as the boundary. Nothing will be re-cut below it.

[wms]

HU,
In your post on milling down to certian level, you are working to HARD.
There is no need to add extra surfaces.

All you need to do is when you get to the section in the tool wizard that ask for automatic extents options is to uncheck the automatic z offset. This will ungrey the z offset option boxes. Then you can enter the depth that want to be z bottom of job and OneCNC will only mill down to that level.

[HuFlungDung]

WMS, I'll certainly keep that in mind, but without trying it out, I cannot be sure if I tried that and didn't like it for whatever reason.
Hmm..... the ideal method would result in rapid moves across the bottom where no machining is intended. Do you know off the top of your head if any method can do this?

[wms]

HU,
I don't know if what you are asking for is possible.
Do to the fact that the program for safty reasons only makes rapid moves at clearance. And I can say I under stand why.
Thats not to say that I don't agree that it would be nice to do it exactly the way you are suggesting. I think that to error on the safe side is probably the way to go.
I have myself made the mistake of tweaking code only to find that now the tool goes thru the part instead of around the part. Not good.

[HuFlungDung]

No no, I should have qualified my statement, since a rise to clearance is okay. I'm just wondering whether some methods will cause the tool to feed all the way across the "false bottom"?

[wms]

HU,
I'm pretty dense, do you mean a false cavity bottom or around the outside of an island (for lack of better word)?
If you mean a cavity bottom, it will be machined (ie: feed) just as if your false bottom was in fact the real bottom.
Around the outside would depend on what was in the way(ie: it would see the model parts and not go thru them) so it might go to clearance before it moves.
Maybe I don't understand the question. If not try to set me staight.

[HuFlungDung]

Yes, I mean a false cavity bottom. On behalf of One2000 owners, this would be valuable to know how to make it "skip" the false bottom, by rapids to clearance. The Rest Robot can likely be used in the OnecncXP to accomplish much the same thing.

Maybe Onecnc can also jump in here and clarify this officially, once and for all. But if you know, post away.

[wms]

HU,
I guess I still don't quite understand the question. I told you I was dence.

I'll try to clear up my thoughts.

Let's say you have a cavity that is 2 inchs deep, with tapered or radius walls at the lower half. And you want to use a 1 inch mill to do the top half but it won't fit into the bottom half.

You can set the extent box to a end depth of z-1.0 (or let the program figure out how low it can go)and then when you go back at it with say a 1/2 mill on step #2 you can set the extent box to start at say z-.975 and end at the defalt value(ie: z-2.) or any other value you chose.

That way the 1/2 mill will not recut the area the 1 inch mill already removed.

This work for both Mill2000 and XP.

This applies to solid model not 2d pockets.
As 2d pocket are bound by the outer boundarys that you pick and the software has no way to know that the area under the top boundary differs from that top boundary.

[HuFlungDung]

Visualise something like an egg carton, all peaks and valleys.

If you had already cut the entire 2" deep mold with a 1/2" diameter ballnose and then you wanted to recut just the top 1" of it over again because, say they had cropped the top 3/4" of the model, and reskinned it (its not just a flat plane top, but is 3d), then you would want to save time by not going all the way down to the bottom any more, but would just want to rapid across the open areas until you get to the islands (this is finish cut only), start at 1" depth and come back up and mill the detail on the island plateau. Am I getting close to making myself clear yet?

[Mortek]

Murry,

I don't think this is possible as the program thinks there is material to come out any where withing the measurements of the extents box. As you say maybe the rest robot in xp will do this for you, I don't know nor can I check. You can however set a z bottom as wms said on the last page of the tool wizard, just change the z depth to what you want. I do this all the time as I machine half the part from one side, turn it over and machine the other.
Ken

[wms]

Hu,
I think we are both thinking about the same thing. Just saying it differently.
If you set the extent box to start at Z0 (or some clearance) and
then set the end Z-1.00 it will force the tool path to stay above Z-1.00 and will not machine below that level.

If you use z level finish it should retract to clearance and move to the next peak or valley.
If you use z level rough it will asume that there is material everywhere (ie: solid stock) and will machine it that way.

HU, kind of like this?

[Mortek]

wms,
bingo, couldn't have said it better myself.

Ken

[HuFlungDung]

I get it now I think, when you said use Z level finish. I got caught on that again.

[wms]

Applicable versions of OneCNC:
OneCNCXp all types

Description of situation or difficulty:
Special user setting for different work

The solution was:

I got to thinking about the user setting and how to apply them to different kinds of jobs rather than different users per say.

For instance:
Mold work setting could go like this:
user name:molds (you could set up different types of mold too)
Then you could customize the setting to fit the work.
Layers = top plate
bottom plate
pull pins
counter bores
top cavity
bottom cavity
reverse ingraving
ect.........

you could even edit the tools and material library to match the work.


aerospace work setting.
user name: aerospace

Layers = stock
webs
material counterbores
ods
bores
tabs (to be removed)
ect......


High speed milling setting.
user name: high speed milling

layers =


This setting would be a good place to edit he material setting to reflect high speed milling parameters as they are so different from regular miling.

These are just examples of what you could do. It's the idea I'm trying to present here. That you could save yourself some time and trouble if you do different types of work, by setting up different setting to match the work.

[HuFlungDung]

That sounds like a good plan, WMS, but where do you see the option to set up several different individual user settings within the program? I must have missed that part.

[wms]

Hu,
It's when you first open up OneCNC from your desktop. (XP only)

[HuFlungDung]

Bear with me, but you mean the little drop-down dialog that says default? How do you change it to something different? Is this referring to default user?

[wms]

HU,
Thats right . You can set up different "users" at this drop down, each will have it's own unique setting. That is, different layer structure, material list, tool setting, color choises, tolerance, toolbar docking, ect....
Basically any thing you can modify in OneCNC.
Pretty cool.

And so you don't have to start from scatch, you can copy your personal setting and rename them to the new acount. Then modifiy the things you want to change.
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)