[Strip]

On the first operation of a part I need to face off 1/16" of 6061 aluminum. I am using the Tormach 1 1/2" facemill to do this operation. Let me say I am new to CNC so please dont call me an Idiot. lol. I have a few questions about this. On my first attempt, I could not find a way to have the mill start off of the part and lead into it. so it ends ip gouging pretty bad. Also, cutting .0625 in one pass at 5100 RPM and 4 IPM proved to be way too heavy for my machine. Maybe because it is starting on the part therefor causing it to cut with the backside of the tool for a small distance. Please advise me on how to get this to lead in and what would be your suggestions for feeds, speeds, and depth of cut. I really need to get this operation running optimum.

[CadRhino]

I do those all the time and at the same feed/speed.
Make sure your plate is secured evenly bit not eccentrically so that the plate bows. This will introduce chatter.
I always start my face milling with the fm a min of 1 3/4" from plate so I enter and exit the cut from the side.
What machine are you using?

On the first operation of a part I need to face off 1/16" of 6061 aluminum. I am using the Tormach 1 1/2" facemill to do this operation. Let me say I am new to CNC so please dont call me an Idiot. lol. I have a few questions about this. On my first attempt, I could not find a way to have the mill start off of the part and lead into it. so it ends ip gouging pretty bad. Also, cutting .0625 in one pass at 5100 RPM and 4 IPM proved to be way too heavy for my machine. Maybe because it is starting on the part therefor causing it to cut with the backside of the tool for a small distance. Please advise me on how to get this to lead in and what would be your suggestions for feeds, speeds, and depth of cut. I really need to get this operation running optimum.

[Strip]

I am using a Tormach 1100. What operation do you use in sprutcam to get the fm to start off of the plate. Do you cut the full .0625 in one pass?

[CadRhino]

I use 2d contour
I mostly do .03" passes but do 1/16" without a problem unless the metal is not supported well.

I am using a Tormach 1100. What operation do you use in sprutcam to get the fm to start off of the plate. Do you cut the full .0625 in one pass?

[Strip]

I use 2d contour
I mostly do .03" passes but do 1/16" without a problem unless the metal is not supported well.

Thank you for replying. I guess since my stock is wider than the 1.5" I will have to go in and physically draw lines for the tool path? This will be terrible since I really dislike sprutcams drawing tools. I guess I will have to figure the stepover in to these lines as well. How much step over do you recommend?

[MichaelHenry]

If you use SprutCAM 8, this tutorial may be of interest:

https://www.youtube.com/watch?v=GB3C0v38DFY

SprutCAM 10 will be released within a few months and has a specific operation for surfacing that should make this much easier. However I usually just face mill or fly cut manually, either with the jog pendant or with manual commands through the MIDI. Also, I haven't checked yet, but PathPilot (Tormach's fairly new controller may have a conversational wizard for surfacing.

[CadRhino]

I draw all of the lines in cad first and use .05" step over

Thank you for replying. I guess since my stock is wider than the 1.5" I will have to go in and physically draw lines for the tool path? This will be terrible since I really dislike sprutcams drawing tools. I guess I will have to figure the stepover in to these lines as well. How much step over do you recommend?

[mountaindew]

Another possible solution is the finish drive operation with settings that work best for your tool type and desired results.
Your limited to a single pass full depth cut for the most part. There are some drawbacks to this and care must be taken to set everything correct or tool paths might not be generated and or it is easy to get tools going the wrong direction.
Still with some practice and care I found this to be very usefull and a way to avoid following limited pre-drawn lines

Copied right from my notebook
Attachment 292196

Flycut setup using Finishing plane operation shown below details a way to build same operation with no lines required and you have complete control over size ,approach, departure , angle, axis to get desired finish and control swarf direction even.

Attachment 292184

First create a Finishing drive operation in the coordinate system plane your working in. Select and or define the surfacing tool "in this case a fly cutter" Then check or set feeds and speeds.

Next to setup and control tool paths first set the lead in and lead out to provide tool clearance before start of cut and at end. This example uses .5 inch to generate tool paths half an inch past the end of the part on both approach and at end.



Attachment 292186

Next Select strategy tap and set milling type, Step and angle. These can be modified to provide right to left, front to back or angled path over the surface to control your finish or where your chips fly. The example above sets conventional milling with 80 % step and 0 angle. These settings duplicated the above 2d example with no lines and this can be changed as desired.

Attachment 292188

Note same operation changing only the angle under strategy changed the tool paths from right to left to back to front. Using this operation and parameters many different tool paths can be generated with no lines that you would have to draw in those locations using the 2d method.

Attachment 292194

One more example of the tool paths set at 45 deg angle shows how many ways this can be done and have decent control of tool paths just by changing a few settings. Note tool paths in yellow above .



As noted above some of these operations when adapted like this can be flakey to use and care must be taken to avoid tool damage!

Hope this helps some users!