LinkBack URL
About LinkBacks
what control are u using it sounds like you might have a tool offset issue
| | |
Here is what I have done
I set my top of part at 0.75(wood thickness), and set my cut depth at 0.125
I zeroed my Z axis on the machine tabletop and then regenerated my toolpath in Mach 3.
I started the cycle and it cut 1/2 in deep instead of the 0.125
What am I doing wrong
On another note, I zeroed the Z ontop of the wood and regenerated the toolpath and started the cycle and it did not reach the wood, it looked like it was 3/4 to high, I have zeroed it out on the table top to onetime and it did not touch the wood when the cycle started.
Could some please explain to me the process when you edit the toolpath, most of my material will be .75 thick, Do I set the top of part to my wood thickness? and then zero out the tool tip on the tabletop. I am new to this does the V23 take into account the overall length of the bit, if so how far should I put the bit into the collet and should I measure what is left sticking out from the collet to the tool tip. This stuff is driving me crazy, I have the training videos and one some of the 3D machining they leave the top of part at 0.000 when they edit the tool path and one others it looks like they set it for the material thickness.
When I create my stock, it ask for length and width but not thickness, I see to the left of this it has the x,y and z origin, what goes in there?
what control are u using it sounds like you might have a tool offset issue
sorry just re read your post mach 3
do you have your tool offset on
Hi csmoak25,Originally Posted by csmoak25
Lets start with something very simple. A flat plane. If you make a rectangle plane at some size of x and y, at BobCads z 0. a 3d toolpath will have a bunch of x and y values and be cutting at Z 0 with rapid planes at the value specified in the features edit dialogue.
If you are toolpathing 2d geometry, you will set a depth of cut "from the 2d geometry" for that particular feature. Say its a circle profile. If the circle is drawn at BobCad's z 0, then a profile feature with depth of cut set at 0 was added, the tool will make a circle a 0. If the depth of cut was set to .5, it would make the toolpath at -.5 down from zero. If the circle was drawn at BobCad's z -1, and the profile feature had a depth of cut set to .5, then the gcode would be outputting a circle at -1.5.
You dont have to tell BobCad how "thick" the stock on your table is. You can put a piece of 3 inch thick aluminum or wood on your machine table, then touch off the top of this as Zero. This will then be the equivelent of the "Zero" in the BobCad workplace.
If you want to have the part in the BobCad workplace be "above zero", and have the zero be 1 inch down from the top of part, then you would want to set the zero on your machine to be 1 inch below the top of the stock you place on your table. Because when the toolpath starts to make it's first cut on the part that was at z +1 in the BobCad workspace, the gcode will be outputting z+1! So if you touched off the "top of your stock on the table" as Z0, then run that code, the tool will move up one inch above the stock and start to cut air.
A best practice to start with to get your head around it, is to draw all your stuff at "zero and below" to start with. Then touch off the actual stock in the machine at the "top of that stock and set that to zero.
If you need more explanation, I'll try to put something more together a bit later..
Burr
Burr, I tried this statement below in 3d, and I get the Zero warning in Bobcad when I am editing the toolpath. Is there a setting in Bobcad I am missing, to ensure I am drawing at Zero
The rapid plane setting has puzzled me to, when I cut 2D if it is set at 0.1000 then my tool tip cuts through my piece as it moves across the stock so I have been raising the rapid plane a bit in 2d and it does fine. What would be a good setting for it when cutting the 3d, most of my stock will be .75 thick
A best practice to start with to get your head around it, is to draw all your stuff at "zero and below" to start with. Then touch off the actual stock in the machine at the "top of that stock and set that to zero.
here is the file
So csmoak25 was working with a BobArt surface as his geometry. The BobArt surface was created at Z 0 and was an "add emboss", so it was protruding above zero. What we did was to right clcik the BobArt item and choose "create/modify stock" and move his surface down by the embossed value. We left the top of part in the feature edit set at 0 now. What this did was to create toolpath and gcode for his surface that runs from z0 and down, leaving all the rapids and toolchange and start and stop of program values at z0 and above. Then we can set the z0 on the machine at the top of the stock to be cut and have the tool work down into the material to cut the part, leaving all the machine moves above z 0.
I created this eagle using BOB Art, however when I run the file it is cutting in 2D, you can tell when you compute the toolpath that there is not enough of it for to be cutting an emboss image
Hey csmoak25,
Your emboss is .25 deep and you have set a cutamount of .22 which is basically 1 pass for the toolpath. This is what the toolpath looks like with a cutamount of .02:
Also one thing to look at is you have set a .5 ball as the tooling for the feature. With this large of a tool, you will see that the toolpath wont go down very much into the wing areas. Try setting a tool size of 1/8 basll and see how the toolpath goes deeper into those areas. You'll want to set the tooling to fit into all the areas you want cut.
Also consider doing some sort of roughing to remove the material before you do the z-finish on it. You could run a slice planar with the larger tool and leave some amount, then add the z-level to surface the finish on it.
Your emboss is very nice by the way. Thats a great result!
Wish I could find a tutorial to walk me through design to cut using Bobcad and Mach3.
Posting Permissions
| | |
