Machsupport Forum
G-Code, CAD, and CAM => LazyCam (Beta) => Topic started by: N4NV on February 23, 2009, 10:39:01 PM
-
The attached file will be for a flywheel's spokes. The DXF is the actual size. I need to offset to the inside so they come out the proper size when I cut them out. When I select all the chains then do offsets using my 1/4" end mill, LazyCam only adds two of the 5 offsets. If I choose a 3/8" end mill, LazyCam does all 5 offsets. Any guesses what could be wrong?
Thanks
Vince
-
Hi, Vince
Well I can get it to offset one at a time, Hears the LCam file's for you to work with, LCam still has allot of issues.
It's late, Chip
-
Here is what I get when I try.
Vince
-
Hi, Vince
Hears a LCam file that all you'll need to do is setup your tool and post I think.
Also a couple pic's and a G-code test file.
Hope this Helps, Chip
-
Hi, Vince
Hears a LCam file that all you'll need to do is setup your tool and post I think.
Also a couple pic's and a G-code test file.
Hope this Helps, Chip
The code is nice and I can use it, but it does not help me figure out why it will not work on my machine. I tried the exact same settings as you and LazyCam will only give me the bottom and top left offsets. I would hate to have to depend on others every time I try to use the program. Without any type of CAD CAM program, it is either hand code or LazyCam. I guess I could do the offsets in AutoCAD and then just have LazyCAM do tool path.
Vince
-
Hi, Vince
Your "I guess I could do the offsets in AutoCAD and then just have LazyCAM do tool path" is the way to Go.
It hasn't been worked on for over TWO years, We keep hoping it will be finished/worked on at some point again.
Moving lead-ins around sometimes helps, But ever when I got it to offset, The posted G-code had errors.
I offset the dxf in cad and used LCam to post it in my previous post, If you'll PM your Phone # I'll give you a call if your in usa or ca.
Thanks, Chip
-
Now that I know how I have to do the drawing, it's no big deal. I made the offsets in my AutoCAD drawing and did an array in under 2 minutes. Sometimes it's just easier to draw the part as shown and let the CAM do the offsets. It's still easier than coding by hand.
Vince
-
Vince - I was able to produce the following offset for your drawing without any problem. In LCAM go into the Setup Function and select "Loading Functions - AutoClean Settings. In that screen you will see a section labled "Connection Line Tol. Used to Optimize." I set this to .01 for this drawing (the setting can be adjusted to accommodate other drawings and needs). A large setting for the here will result in your "slices," being joined which makes offsetting a problem. For the offset I used a .125 endmill and assumed you wanted to offset to the inside of your spokes.
Although I did not cut the project, I did use LCAM to produce the code. It appears to be right. LCAM did produce one errant circle that had to be edited out. The entire project, loading into LCAM, changing the Optimize setting, offsetting, generating the code, and editing the final gcode took about 5 minutes.
Don't know if this will help or not. But, I have used LCAM to produce some very complicated pieces and felt tackling your problem would be fun.
Good luck with your project. Post a completed picture when you are done.
Bob@BobsShop
-
Bob, I tried changing the setting. I tried .1, .01, .001, .0001. As a result I was only able to get 3 of the spokes to offset. I'm still going to draw with tool part center instead of actual part, but I would like to know why it works for some and not others.
Vince
-
Hi Vince,
I tried your DXF and discovered that if the selected tool is too large to cut an arc at the corners, (tool rad. = > part rad.) then there is a problem. By selecting a smaller tool, it works fine here.
Are you trying to use a .25 cutter ?
Might help,
RC 8)
EDIT: I see in your first post now......1/4 and 3/8 tried. I think tool rad. smaller than the drawn rad. is the answer.
-
Hi Vince,
I tried your DXF and discovered that if the selected tool is too large to cut an arc at the corners, (tool rad. = > part rad.) then there is a problem. By selecting a smaller tool, it works fine here.
Are you trying to use a .25 cutter ?
Might help,
RC 8)
EDIT: I see in your first post now......1/4 and 3/8 tried. I think tool rad. smaller than the drawn rad. is the answer.
It works for a 3/8" tool which is larger than the radius. It may be that it does not work if the tool radius=drawn radius.
Vince
-
Quite possible......sometimes.....for some folks.
I didn't try larger tools as they would not cut the desired profile.
Can you verify for me that it works OK with a smaller cutter ?
Thanks Vince,
RC
-
Quite possible......sometimes.....for some folks.
I didn't try larger tools as they would not cut the desired profile.
Can you verify for me that it works OK with a smaller cutter ?
Thanks Vince,
RC
It works for anything smaller than 1/4" and larger than 1/4". There must be a problem with the code when the cutter radius=drawn radius.
Vince
-
Vince, now that you mention it, I remember encountering a similar problem. In my case, I cheated and told LCAM the tool was .001 (or something near that) smaller than the actual tool. As I recall that solved the problem. Another writer said LCAM has some issues; And it does. But since I am not building orbital rockets and LCAM has enabled me to cheaply make one-off parts for the Harley, I give it some slack.
Bob@BobsShop - Making parts and grinning.
-
YES BOB !
I vaguely remember reading about that also.
Been a while.....forgot to write all of these tricks down.
Thanks for the memories,
RC
-
Thanks Bob, I just tried it with a .249" tool instead of .250" and it works.
Vince
-
Promise this is my last post on this subject. :-\
Just because I am getting older (a lot) and even more forgetful, I decided to try one more "fix," to avoid this type of problem in the future. I went in to my tooltable and added .0001 in the Diameter Wear column for every tool. Tried the DXF file again with a .25 endmill and LCAM produced the code properly.
The .0001 wear lie should not cause many problems for the type projects I am contemplating. If the adjustment is a problem then Mach3 and my Taig mill are a lot more sensitive than I ever imagined.
Bob@BobsShop - has left the building.
-
Nifty trick Bob...
Thanks,
RC
-
This discussion is exactly what I was looking for in the Yahoo Groups (and didn't find). I thought I would have to buy a separate Cam program to do offsets but apparently not. I'm putting together a Taig system to cut sections out of brass plate to create clock wheels. I need to cut inside the line for the spokes and outside the line for the perimeter of the wheel. Can I do both at the same time with the same drawing or do I need a drawing with two layers? Do I need the Pro version of LazyCam? The last thing I want to do is create drawings for the toolpaths.
I've been playing with the demo version of Mach3 for a few months as my steppers and other parts come in and apparently LazyCam is also a demo and won't show offsets with my drawing.
Another related question. I have to mill a spoon-shaped so-called click spring. The handle is 3/32 high but the spoon end is 1/16th. I could do two drawings but would rather do one. Does this call for two layers to the drawing and could LAzyCam help here too?
-
Two possible solutions - Invest in LCAM Pro or look into D2nc link is http://www.d2nc.com/ An inexpensive program that should do just what you want. I use both programs depending on what I am doing at any given moment. Graham Hollis of D2 has give me excellent support in the past.
Like most (if not all) inexpensive programs LCAM and D2 each have their own set of quirks, but I have been able to work through them and (IMHO) get excellent results.
Bob@BobsShop - not affiliated with anyone -