2-axis cut control - Speed/feed calculator RPM too high

[Neil_J]

Hi,

In the 2-axis cut control window (see pic), there is a button to calculate speeds and feeds for the tool and type of material selected....

My problem is that it wants to set the RPM way too high for my machine. I don't see an option anywhere to set the max RPM. I have been setting the speeds/feeds manually for a while, but it would be nice to use this feature.

[scubanick]

go and change the surface footage for the material you are using
and for the chip load for the tool and save them
that way when u go back to that material and tool
it will be where u want it

[hawaii500_1999]

i've had the same problem but i gave up on trying to set a max rpm and just enter in the speeds and feeds myself.

i use the calculator on the robbjack website a lot http://www.robbjack.com/

[championp]

Generally, if you retype the RPM to your machines max, it will update the feed to maintain the same chipload (auto calculate). It will also keep this info if you use the same tool for two consecutive operations. Sometimes when machining 6061 I tell surfcam it is 2024 to keep the speeds and feeds more realistic. I think surfcam speeds, feeds, and stepovers are a little too aggressive most of the time (default depth of cut for a 2.5 inch facemill is .990, with a finish pass of .099).

If you want to use the same parameters from a previous setup automatically, in the operations manager you can click on the previous toolpath-edit parameters- and hit cancel. then after picking your geo it will come in with the same tool#, size, offset, speeds, feeds, stepovers, stock to leave,etc.

Or copy the previous toolpath, paste in the next setup, and regenerate and reselect geometry.

Chris

[Neil_J]

Originally Posted by championp Generally, if you retype the RPM to your machines max, it will update the feed to maintain the same chipload (auto calculate). It will also keep this info if you use the same tool for two consecutive operations. Sometimes when machining 6061 I tell surfcam it is 2024 to keep the speeds and feeds more realistic. I think surfcam speeds, feeds, and stepovers are a little too aggressive most of the time (default depth of cut for a 2.5 inch facemill is .990, with a finish pass of .099). If you want to use the same parameters from a previous setup automatically, in the operations manager you can click on the previous toolpath-edit parameters- and hit cancel. then after picking your geo it will come in with the same tool#, size, offset, speeds, feeds, stepovers, stock to leave,etc. Or copy the previous toolpath, paste in the next setup, and regenerate and reselect geometry. Chris

Thanks, I think that just answered all of my questions... Any more tricks you can share?

[championp]

I'm sure I have few tricks left but you will have to ask specific questions so I know what to say.


Chris

[Neil_J]

Originally Posted by championp I'm sure I have few tricks left but you will have to ask specific questions so I know what to say. Chris

Any tricks relating to engraving text? Right now I am importing the text, using the Edit/Text to change from zero-width to TTF, then using the Edit/Text/Explode, then 2 axis / pocket. I haven't found a way to engrave zero-width text (i.e. only engraves one line per stroke).

Thanks...

-Neil

[championp]

For text I use the 2-d contour and cut "on" instead of climb. I usually change the color of the text so I can use mask and select "visible" . I use no lead ins or lead outs. For engraving a surface I use 3d project then transform/rectangular array in the z axis only to get to the desired depth with depths of cut. Sometimes you can click "calculate z values" in the project box and it will put out the z depths automatically.

Chris

[protogregg]

I reset the defaults in SurfCAM for a safe stepover and step down in the tools>options>NC Defaults>2 Axis: Side and depth roughing size change to 0.6300/Cutter radius, Finishing size (Side and Depth) change to 0.0788 Cutter Radius. That ratio works well for metric, I can't remember what I set it to for standard increments (but it was very close to the same ratio). This will default a very safe stepover/stepdown, which can then be adjusted up for ABS, Ren, etc.

[tnik]

you can edit the post processor to only allow a max rpm..

if [Speed] > 7500
S7500 M[Direct]
else
M[Direct] S[Speed]
endif

Now, thats for mpost, not spost, and as for adjusting the feedrate automagically with the post, I'm sure it can be accomplished, but I haven't tried it yet..

[camaru]

When engraving stick figure text you need to make a couple of changes.
you need to use contour2d, on the cut control page set cut method to "on" and while you in the contour 2d process pick the "options" tab and set gouge check to single. NOTE when you are done, set gouge check back to full and cut method back to climb or conventional.