Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: kolias on April 17, 2011, 10:21:55 AM
-
There must be an easier way to do a pocket….
Lets say that I have a piece of lumber 12”x 12” and in the center I want to cut an intricate design that is 6”x 6”. Since the design is intricate I will use a 1/32” bit to be able to get all the small details.
But when I create a pocket with islands checked, it will take forever to pocket the area around the design with the 1/32” bit.
Although I don’t know how to do it yet, I know that there is a command which allows for a tool change. So lets say that I will use a 1/2" bit to start the pocket but when it comes too close to the design this bit is too big for the intricate design and I will have to change it again to a 1/32” bit.
How do I find in the gCade where I have to issue the tool change command to change from the 1/2" bit to the 1/32” one?
The M-Codes for the M6 command says “Tool Change (by two macros). Where do I get these two macros?
So when I find the right place in the gCode what I put there? Just M6?
-
I think what your after is called rest machining. That's something that has to be figured out by your CAM software. What happens is that you start with a large bit and work your way down. The first passes will be with the large bit to quickly remove material. The next size smaller will go in and machine the parts that the larger bit could not get to. If you go even one step smaller, it will machine details that the previous pit could not get to.
All of that is calculated in CAM. It's not just a matter or dropping an M6 tool change command in the code. What are you using for CAM? I know some of the lower cost CAM programs aren't capable of this.
-
The toolpaths for a 1/32 tool will be different than those for a 1/2" tool. As was previously mentioned, you can't just add an M6.
V-Carve Pro (and Aspire) allow you to specify a larger clearance tool along with the standard smaller tool. Two separate toolpaths are created, with the larger one first.
Here's how to do it with more basic software.
You need to draw separate pockets and islands for each tool.
For the 1/2" tool, make the pocket about .02" smaller, and the islands about .02" bigger. Create the toolpaths for the 1/2" tool with these.
For the small tool, you'll use the regular pocket outline. But, for the islands, you'll want to offset the pocket enough to get any material that was missed by the 1/2" tool. Depending on the design, it can be as little as .04", and as much as 1/2", or maybe even more. Use the original pocket and the "offset island" for the toolpath with your 1/32" tool.
Hope this makes sense.
-
I use LazyCam Pro as my CAM which is enough for now to get me going learning. I didn’t know that a CAM program will make allowances for the pockets with different bits but there are many things I don’t know and I discover them as I go along. I’m only doing hobby work with my CNC and it’s interesting to discover and learn new ways to work with
Gerry I will work with your guidelines and I think it will be easy to do it
Thank you both
-
Nicolas,
LC is fine for offsetting, cutting out a profile, and "basic" pocketing. If you want to do fancy stuff then you need different software expecialy for 3D stuff.
That software is anywhere from say $200 to $2000, so once you decide then you pay the price.
BTW,
Thought you were taking a look at all the different software available......I was wondering which one you would select ......
gets old after a while! ;) :D >:D
RICH
-
Yes I’m still looking which CAM software will be good for me but first I must learn a CAD software; I mean no matter which CAM I will get it will do no good to me if I can’t make my own drawings.
Right now I’m practicing my skills with Inkscape (thanks to Gerry) and looks good and progressing all right. LC Pro also helps to learn some techniques and see the results in actual cuts.
When my skills improve and I’m ready for a better CAM, then I will be in a better position to buy one. Right now my choices are V-Carve Pro, Cut3D and SheetCam but by the time I’m ready to buy this may change.
However with the summer almost here there is lots of work outside and somehow I suspect that the CNC will be in the backburner for a while. For us up north, CNC is a fulltime winter project and only a part time project in the summer LOL
But I’m getting there RICH, slow but steady……
-
One thing to consider, is that with V-Carve Pro, you can do your design work and CAM all in one. Most V-Carve Pro users son't use any other drawing programs, as it has all the tools built in.
So, you might spend a lot of time learning a drawing program, end up buying V-Carve pro, and have to learn to draw in that.
However, learning as many programs as possible only helps. And If you do go with V-Carve pro, you can always import from other drawing programs.
-
Also...As much as I love SheetCAM for plasma work, it can not do rest machining. If that feature is a must have, keep that in mind.
-
Good points Gerry
At $600 V-CravePro is pretty expensive for just hobby use. So if Inkscape can do the job for me than I may only consider Cut3D which is half the price.
rrc1962 what do you mean that SheetCam can not do rest machining? Which feature is that?
-
Rest machining is what you're trying to do. Machine using a large bit to remove the bulk of material, then come back with a smaller bit to get what the large one couldn't get. Imagine you have a simple pocket with 1/32" radius corners. Using rest machining you can run a large bit, like 3/8" first to clear most of the material, then follow with a 1/32" bit to finish the corners. The toolpath for the 1/32" bit would only be generated for the portions of the part that the large bit could not machine due to it's size....IE: The corners.
Gerry explained how to do it manually. Most 3D CAM programs do this automatically. SheetCAM is 2/2.5D which is pobably why it doesn't. In ArtCAM, you just list the tools you want to use from larges to smallest and it figures the toolpath for each tool automatically.
-
Thanks for the info rrc1962, very good to know
-
To do "rest"machining for your profile try this.
Offset 1 -Make an offset of the profile for cutting the profile outline using the small end mill.
Offset 2 - Make an offset based on a larger end mill of the profile. When done it should make a path that it can cut, thus it will not get into tight spots.
Now you pocket offset 2.
Now use select offset 1 & 2 and pocket the inside with a tool.
Now cut the profile based on offset 1.
I don't know what your profile looks like.
Fool around with the above in LC.
Sometimes LC pocketing leaves something to be desired!
RICH
-
Keep in mind, "rest machining" is not absolutely necessary. If the CAM program is not capable of rest machining, you will just have to re-cut the entire machined area with the smaller bit(s). Rest machining simply picks out only the details that were un-machinable with the larger bit, and cuts those places only. It cuts the "rest" of the material. This makes machining time go way down in some cases, but for the weekend warrior, it's not a "must have". Personally, I like cutting across the entire project with the last bit. I think it gives it a more uniform , and appealing look. If I found a CAM program that I liked, but it didn't have that function, I would not discard it on that fact alone.
-
I like what you said RICH and I will give it a try. Never thought to make Offset 1 & 2 like you said, very smart and I’m sure it will work.
That’s me Sam a “weekend warrior” with lots of time available LOL. I agree with your techniques and I also agree that choosing a CAM program it is a difficult process and not all features may be available on the one I will like
Thank you both