I need to create an offset around the outside of this shape using a 1/8 inch cutter. I can offset the inside of the shape just not the outside. I have tried the usual tricks but I cannot lose the 0,0 point because i dont know how to get it back to exactly where it was.

Thanks in advance

Steve

Have attached two different files - both offset .0625 (1/2 of .125 end mill) to the outside.  Did not change the 0,0 orientation.

One of the files was written in CADX11, the other in AutoCad 2008.  Not sure which format will work for you.

Offsetting to the outside was not a problem with either program. CADX would let me select your dxf as one continuous chain and offset it that way.  AutoCad required selecting the different segments and offsetting individually.  In addition, I also pulled the file into LCAM and also was able to offset with no problem.  I may not have understood what you were trying to accomplish.

Hope one of the two will work for you.

Bob@BobsShop

No, you understood just fine. For some reason Lcam wont do things on this computer that others have no problem doing. I have been trying to do that simple offset for 3 days now. Lcam would offset to the inside but not the outside. I am very new so i have the latest version. Maybe i should look for a little bit older version of Lcam.


You did the offsetting right in auto cad?  Can autocad 2002 do that? If I could do simple things like that in cad it could have saved me alot of time.

Thank you so much!!

Steve

Don't know about AutoCad versions before 2008.  That was the first time I ever used it.  The CADX11 program is a free cad program that I use for some things that AutoCad won't let me do - one of them is importing DXFs of engraving fonts.    The free program has no time limit, but it does have a file size limitation.  As I recall the free version would have handled the file you posted without any trouble.  I did eventually purchase a full version, but by the time I got around to it, I was dealing with some pretty large and entity intense programs.

CADX can be found at www.graytechsoftware.com/

Oh, I failed to mention, but I am sure you noticed, I did not delete the original drawing after doing the offsets.

Good luck with your projects.

Bob@BobsShop  is not associated with any software or hardware companies.   For what it is worth, I am not associated with anyone!

"Lcam would offset to the inside but not the outside"

STEVE,
I have run across that jusr recently and in fact just now with your posted DXF.

So here are a few tricks:
1. Create an inside offset with 1/8" cutter
    Then i unenabled the original outline
    Then i created an outside of the first offset with a 1/4" tool
    which gives the same ( i think, would need to check the radius's  ) as if you offset the original with a 1/8" tool

2.For some reason, sometimes you just can't do an offset because of the radius. So for this one i just did an offset
   using a .2" dia and got an outside offset. Then i deleted that offset.
   Then i used the 1/8" tool and it worked just fine.

3. Sometimes when things just don't seem to work out. Close and re-open LC.

Nope, i have no explaination why the above works.  No this is not in the manual.    Because until your file and another two i helped recently, i never had the problem. 

RICH

Thanks Rich!

Tomorrow we cut parts!!

Hi Steve,
  Just to add to the confusion..........here is another simple workaround. If you don't mind lying to your machine and coping with a .0005" error.
 The radius's in your drawing match the .125 cutter exactly.......this is what causes the problem.
If you set the diameter of the .125 tool in the tool table to .1245 or .1255 it will offset correctly. (actually, .1246 and .1251 works here)
LCam has always been picky when tool rad matches a profile rad exactly.
Good luck,
Russ  

I had no idea.

When i draw a part from this point on i can make the fillets a thou or two bigger than the cutter.

I did get the pattern cut today so i can get the parts poured. Going to be aluminum castings for a model aero engine.

Thanks again!!