Using Aspire, generating G-code for a project, everything in the code looks good, both rough cut and finish paths. My rough cut is done and looks great, didn’t notice any issues. However, I just stopped the finish cut on 3% in due to the tool paths being so far off. A giveaway was the rocking motion the entire machine was doing when the X axis motor would change direction. I got up close and watched the change of direction, and the X axis motor doesn’t stop and change direction smoothly, it jumps, continues, and jumps and changes directions erratically, causing the machine to lose Zero. I reset the machine, re-homed it, reset the settings, and began the cut again with no change. Upon cancelling the cut, the machine returned home and was off by 1/2" left. I just cut some letters earlier no problem. Machine has been working flawlessly for the most part, and I use Aspire for everything.
3D Finish 1.gcode (1).nc (7.9 MB)
Machine settings are as follows:
Dis-engage the X-belts, does the carriage run freely with uniform friction?
How tight is the belt?
Check and double check whatever set screws you have on X.
Your ballnose looks like it has heat damage. Is it HSS or Carbide? On the video it looks like you are asking the ballnose to remove a fair chunk of material which can cause loss of steps.
That’s a Spektra bit from Amana tools. Comes heat treated, looks normal.
It looks like the chunky part of the ballnose is hitting the steep walls, the software won’t account for the tapered geometry of the bit, try having a larger vector offset for your roughing pass to account for this, 1/4 inch should do it.
Good point. Right now my offset is low, .04 , Does that account for the motors losing steps and jumping?
Edit: Just changed it to .25 and got this warning message. Were talking about the Roughing pass, correct?
Set the machining offset to 0.03 for the finishing pass and set the boundary offset to a little over half the bit diameter. I use 0.13 for the boundary offset for that bit diameter.
For the “machining offset”, are you inferring not to use a raster cut pattern, and keep it set to offset? Yesterday was the first time I experimented with raster, and it was also the first time I experienced this problem.
I think he meant ‘machining allowance’ to 0.03
Yes I meant the machining allowance.
I agree, I would use boundary offset on roughing pass to 0.26 and boundary offset on finishing pass to 0.13 as Randy suggested. (assuming 0.25 tools)
you need a bigger boundary offset on roughing than finishing to allow for the taper
With a boundary offset greater than the tool diameter for the roughing pass, you may end up not leaving any material for tabs if you are using them. Use the toolpath preview to verify your roughing pass.
The boundary offset and machining allowance I suggested were for the roughing toolpath. The boundary offset for the finishing toolpath should be approximately 1/2 the tip diameter plus a little bit. For a tapered bit you can probably use the tip diameter.
Thanks for all the input guys, this is my first attempt at a 3d carve. Here is the preview and settings for rough cut.
Your preview shows the tool cutting through the material around the numbers. Is that your intent?
Yes, that’s how the actual badge appears.
Good News, after the minor adjustments this morning regarding the offsets//raster/ clearance, seems to be cutting on point now. Just did a test 3d carve in some plywood and it looks great. Thanks for all the help!
Please post your results, i’d like to see how it turned out.