Surface Toolpath Issue

[TeccBoxx]

Trying to do a simple surface toolpath and I have havving a bit of a problem.

 

I have a 2 inch half cylinder cut through a block and when I toolpath it it is leaving a step on the bottom of the cylinder. I have used both surfaces and solids, tried parallel, pencil, and scallop toolpaths and they all give me the same thing.

 

I would just stand it up on end but I have no tool long enough to bore it out.

 

Here is a picture of what I am trying to do, where the scribble on the bottom of the part where the toolpatch is leaving a small step.

Anyone have any suggestions?????

[htm01]

backlash in machine or a flat on ball

 

have you tried just a wireframe revolved toolpath?

[Mjölnir]

+1 on wireframe revolved.

 

Or parallel / raster limiting depths to just do the bottom.

[TeccBoxx]

Thanks for the idea guys, it might be backlas, as I have tried two brand new 1/4" ball endmills, and the wireframe revolved was the second toolpath I tried after a parallel off a solid didn't give good results.

 

It is weird as it leaves a peak/step at the bottom.

 

I am trying a steep parallel right now to do just the bottom from 0-20 degrees to see if that will work.

[Mjölnir]

If programed arcs in the X-Z or Y-Z plane(s) (revolved toolpath) are leaving steps at the quadrant where the Z axis reverses direction that's a real good indication you've got mechanical issues with the machine.

[Josh T™]

I would try parallel with the filter ratio set to 1:1, filter tolerance set to .0001 and create arcs in the x/z - y/z axis checked. You'll have to adjust the machining angle to backplot the correct arc structure. This should post arcs instead of linear moves. If there is still a flat in the bottom you may have backlash/look ahead issues.

 

Email me the file and I'll try to help you... it's a slow day here anyways.

 

Josh

[MotorCityMinion]

Perhaps.... Surf Fin Blend it with 2:1 Filter at .002 TT. Examine the toolpath in backplot, you should get nice clean arcs. Code should look good also. If the machine can't do it in YZ, try rotating the part 90.deg to cut in XZ.

[JDowe]

It is one surface right - if its not this

can cause that

[Cad-Camr]

I have had this happen to me before and I ended up creating 2 Ruled Surfaces that overlapped a bit at the bottom.

[heavychevy2155]

If he used the wireframe toolpath, he used wireframe not surfaces to drive the tool. If you still have problems after using the wireframe path I'd say its a mchine issue. Try rotating the part like motor said.