2 1/2 axis Facing on the bottom of a part

[jcdammeyer]

I have to create a customized heatsink from extruded stock. I designed the stock with the stock outline on the XY plane and extruded to the heatsink height. One sketch to remove some of this extruded section for a clearance.
Then a series of repeated rectangles and cut down to a bit a above the XY plane and bingo there was my ribbed heatsink stock with a notch in the ribs.
Now flip it over and create both pockets and posts on the bottom which results in material below the XY plane (-Z direction) and pockets above it (+Zdirection)

I've been able to use my 2017 AlibreCAM to create both the pockets and and the profile the outline out of the stock. But the 2 1/2 axis facing just isn't working. It puts a 0.125 tool into a 0.089 hole. It runs into one of the extruded pads but leaves a larger gap around round posts.

I've run into this before and usually played around until it's sort of fixed but this time playing doesn't work. I'd like to write myself a tutorial so when I want to do this I can refer to what worked before. If I can get it to work.

The steps would be I think:
1. Orient the Machine Tool rotating Z around X so when simulating the tool bit is above the work which is also mounted upside down in the vise.
2. Surface first setting the correct machining regions.
3. Select tool and other parameters
4. Generate tool path.
I've attached the part. What am I doing wrong?

 

[fabcadmz]

See if the attached file works.
I made few changes:
1. I made a new sketch for the facing drive region. I offset the line by 1/2 the cutter dia. from the extruded pad. 2 1/2 axis facing will always put the cutter on the center of the outside profile, that is why it cut into the pad. I also moved the line away from the round post as there wasn't a large enough of a gap to fit the cutter between the line and the round post.
2. I made a new 2 1/2 axis profiling Mop to cut the step on the neck.
3. In the part you posted, the Z cut level was set to top, therefore AlibreCAM considered the level of the drive region as the top of the facing toolpath and cut down from there. Setting the alignment to bottom forced it to project the toolpath up from that plane. See this article on MecSoft's blog: https://mecsoft.com/blog/understanding-cut-levels-in-2½-axis-machining/
4. The reason the facing toolpath was putting the cutter in the hole was because the round edge was selected (DriveRegion1 in machining regions) The software was cutting around the inside of that extrusion.

 

[jcdammeyer]

Thank you.
Because I saw the facing section move the cutter outside the line on the left and right I assumed it was clever enough to also go outside the line at front and back and properly face around both posts. I hadn't realized the software wasn't clever enough to face around the front post and avoid that back pad.

I modified the sample you changed to include facing the area behind the back. Setting the XY zero to the bottom left corner and Z at the highest point then worked for me to touch off on my test sample of MDF board and after a few missteps managed to model the bottom so it's like the 3D printed model.

Next step is to figure out how fast to run this since I don't really know how fast the two flute end mill is turning. The Bosch Colt has a range from #1 to #6 for speed. My JGRO router table can't handle deep cuts ends the 0.015" depth per pass.

I'll re-read the link you posted and see if I can't make myself a better step by step instruction document to be able to do this.
John

 

[fabcadmz]

One thing to remember about 2 1/2 axis operatons is: the 3d model data is not used for toolpath calculations. All toolpath calculations are derived solely from the 2d sketch. You can generate 2 1/2 axis Mops from only sketches without needing to create a 3d model.