Fixturing and toolpaths for noobs

[koenbro]

So here is a one minute video of machining the hitch receiver recovery point.

Oh, and @JimDawson thank you for the suggestion to use SPIRAL for the filleted hole opening (and for all prior advice). SPIRAL operation with Machine Cusps worked real well using a 1/2" ball end mill.

A project like this doesn't require a thou-level precision for the holes, but it gave me an excuse to use the Mesa Tool 1/2" x 3" boring bar.

Quick question: What operation would you use for the flat narrow ends -- I have a Sherline shoulder fly cutter and tried to use FACE but did not work. I ended up using a regular 1/4" endmill but it left grooves. Although for this project it doesn't matter, would like to know for the future.

 

[JimDawson]

Quick question: What operation would you use for the flat narrow ends -- I have a Sherline shoulder fly cutter and tried to use FACE but did not work. I ended up using a regular 1/4" endmill but it left grooves. Although for this project it doesn't matter, would like to know for the future.

Do you mean where the shackel attaches? I would most likely use a 3/8 endmill to rough that out, then go back in with a 1/2 ball to finish. If you're not in a hurry, use the 1/2 ball and do it all in one pass with a 0.005 stepover.

I don't understand why you were left with a rough finish, you would be able to see marks, but should not be able to even feel them when done. Dull endmill maybe? Slightly out of tram? I'll draw that up and try a couple of different cutting strategies, and post them.

 

[koenbro]

The surface is smooth just has the visual pattern, whereas the flycutter would leave mirror-like. Just want to improve my skill set for the future.

 

[JimDawson]

The surface is smooth just has the visual pattern, whereas the flycutter would leave mirror-like. Just want to improve my skill set for the future.

Ahh, well then I would rough it out, finish the fillet with a ball end, then a final cut across the face with the fly cutter. That would give you the tool mark pattern you want.

The other option is to flip it up on the side and cut it with the side of the endmill.

 

[Parlo]

The surface is smooth just has the visual pattern, whereas the flycutter would leave mirror-like. Just want to improve my skill set for the future.

Use scotchbrite on a random orbital sander, choose the abrasive grade to suit the level of finish required. It is extremely quick and gives nice finish options from satin to mirror.

 

[koenbro]

Ahh, well then I would rough it out, finish the fillet with a ball end, then a final cut across the face with the fly cutter. That would give you the tool mark pattern you want.

The other option is to flip it up on the side and cut it with the side of the endmill.

The final cut with the fly cutter would be a FACE operation? I need to select a surface and then oddly, the flycutter overshoots that, meqnaing it goes in farther. I am going to try that again and post the screen grabs.

Flipping it on its side sounds great actually!

Use scotchbrite on a random orbital sander, choose the abrasive grade to suit the level of finish required. It is extremely quick and gives nice finish options from satin to mirror.

Yeah I will have to try that.

 

[JimDawson]

The final cut with the fly cutter would be a FACE operation? I need to select a surface and then oddly, the flycutter overshoots that, meqnaing it goes in farther. I am going to try that again and post the screen grabs.

I think the TRACE function would work for this, or just a manual jog across the face.

Flipping it on its side sounds great actually!

 

[koenbro]

Seems more complicated than I thought . TRACE is shown here:


ADAPTIVE overshoots it as does FACE:

 

[JimDawson]

The TRACE tool path runs the tool center line right down the trace line, much like ENGRAVE. That's the reason I drew the sketch line where I did, and assumed a 2.25'' dia cutter. This should put the edge of the tool right at the front edge of the fillet. Sometimes you have to make some changes to the drawing to get it to cut what you want, then revert back to the original drawing for other features. I use TRACE when there is no there reasonable way to do it.

You can also use a 3D adaptive and constrain the cut area with a sketched box. You can always make it do what you want, but sometimes requires a bit of fiddling.

Here is an example of a 3D adaptive roughing cut

 

[JimDawson]

Here is a real world TRACE tool path. I made a measuring error on the flywheel for my tube polisher project and of course transferred that measurement to the drawing without double checking. No real problem, but I need another 1/8'' clearance in the pinion gear housings.

I need about 1/8 more clearance here.


The left side is what I have now, the right side is what I need


There are several ways to do this, but I chose the simple method and will be cutting some air. I could have constrained the adaptive clearing with a bounding box to reduce the air cutting, but I'm not in that big of a hurry and air chips are easy to clean up.


Then I decided to make a final 0.020 contour pass to finish cleaning up. I could have just set the adaptive clearing to leave 0 stock and not even done a finishing pass, but what fun is that. But when I tried to do a 2D contour it insisted on taking a cut all the way around the part rather than just the face I wanted to cut. I could have constrained a 3D contour with a sketched bounding box, but I insisted on making it do what I wanted with a 2D cut.

This is where TRACE comes in. First I drew a 13.5 dia circle, then offset the the circle the radius of the 3/8'' endmill (0.188) from the surface I want to machine because the tool center line follows the trace line. Then drew the two cut lines where I wanted the endmill to start and end, then trimmed away the rest of that circle. So now I have a tool path to follow exactly where I want to cut.



So now all that is required is to go into CAM, select Trace and select the line. Since the line is at the top of the part, I also needed to set the axial stock to leave at -0.645 to reach the bottom of the area I want to cut because the trace function cuts exactly on the line unless you tell it otherwise. You also can use multiple step downs if desired.



Now I just need to go make some chips.