Side Engraving

[Grimes]

I was messing around with trying to engrave onto the side of a part on a vertical. Could not figure out any way to do it without spending a lot of time manually programming it. Any advice from someone is greatly appreciated. I couldnt even find a tool to do it with, was looking for a ball nose with clearance.

[Colin Gilchrist]

7 hours ago, Grimes said:

I was messing around with trying to engrave onto the side of a part on a vertical. Could not figure out any way to do it without spending a lot of time manually programming it. Any advice from someone is greatly appreciated. I couldnt even find a tool to do it with, was looking for a ball nose with clearance.

Engraving on "the side"?

So you want to take something like a Lollipop Endmill, and have it come from the Top, but cut on the side or front? 

This is the one application where you need a different Tool Plane and Construction Plane. The Tool Plane should be Top, and the Construction Plane should be either Front, Right, Back, or Left, depending on which side of the part has the engraving. 

Use Contour, and Reference Points to get your tool into the cut, and out from the cut. You may have to Toolpath one letter at a time, to get proper Entry/Exit motion. 

I did a project where we had a special wheel cutter mounted to a separate motor, at right-angles to the main spindle. Using separate T/C Planes was the secret to programming that feature.

[Colin Gilchrist]

Are you looking for an example like this:

 

 

FRONT-ENGRAVING_TOP-TPLANE.mcam

[Colin Gilchrist]

The key techniques here are:

• Properly defined Lollipop Mill & Holder
• Project Toolpath > Cuts "on center" of the Curves (wireframe chain) geometry
• Select your Surface, then your Curves. When the dialog box opens, click [Planes], and then set your Construction Plane to "front" or "side". (basically; C-Plane's Z-Axis should be "Normal" to your Surface/Curves for projection. T-plane gives the orientation of the Tool/Machine. C-Plane tells the Toolpath Algorithm > "how to compensate for the sphere that is driving the path motion". In this case, we want 'C-Plane' set to Front, with T-Plane set to "Top"
• Use "Clearance" value for initial/final retract position
• Set Retract/Feed to "0.0 Incremental". This keeps the tool "down" between the chain start points
• Use [Direction] Button on the Surface Parameters Tab, to tailor your Entry/Exit motion from "the start/end point of the chain"
• Set "plunge angle" to 0.0. (Can also use +- numbers, to tailor the vector approach. For example, use -2 degrees, or +2 degrees, to ramp in/out from a tricky area)
• Set "plunge length" to a big number, but make them different (I like to use 2" & 4", for Inch mode, and 50 & 100 mm, for Metric Mode). The reason is it "shows you visually", which move is the entry, and which move is the exit. Then you can play with the XY Angle, to find the correct entry angle, and exit angle. They are typically "180 degrees apart".
• Be aware there is also a setting in "Direction", which allows you to choose the angle "relative to the Toolplane X-Axis Direction", or "relative to the Cut Direction". Be careful with these options. I typically use "relative to T-Plane X" > because if you change the Cut Parameters, with "cut direction" selected, it can totally change your entry/exit angles.
• Use Backplot & Verify to be sure your cutter is going where you want it to, and only moving where you tell it to.

[Colin Gilchrist]

I forgot one:

> Gap Settings Dialog Box > disable two checkboxes that say "gouge check”

[#Rekd™]

3 hours ago, Colin Gilchrist said:

The key techniques here are:

Colin you are above an beyond most of us!!! 

Big thumbs up!!!!

[Colin Gilchrist]

8 hours ago, #Rekd™ said:

Colin you are above an beyond most of us!!! 

Big thumbs up!!!!

I appreciate you saying that, but I'm just trying to pass on things I've learned from the forum and my classes over the years. I can only program so many parts myself. If I can teach others what I know, then they can benefit from the knowledge too. Plus; I just like showing off little used, or hidden functionality.

I've heard people asking "why even have both a Tool and Construction Plane? Just make it one, and it would be less confusing".

Sure, but in an instance like this, it is actually necessary to have them be set differently from each other. 

[Grimes]

im gonna try this info colin, every time i get this job im always thinking "this has to be able to be done".

wtf is a gap setting, i still dont fully understand it?

[Colin Gilchrist]

1 hour ago, Grimes said:

im gonna try this info colin, every time i get this job im always thinking "this has to be able to be done".

wtf is a gap setting, i still dont fully understand it?

When the Toolpath is asked to "cut" the part, it does so by creating 'slices'. Think of a Parallel path, or a Waterline path (surface finish contour). With these paths, you either get a plane like "front" or "side" that is offset through the geometry, or a Z plane, dropped in steps.

Wherever the plane contacts the model, you get motion. 

Whenever you reach the "end of a pass" the Toolpath now has to decide: what do I do? 

This is a "Gap".

Gaps can occur "along the cut path" (like when there is a hole in the surface), or they occur "between the 'end' of a current cut pass, and the 'start' of the next 'cut path'. A gap occurs any time there is a break between cut motion.

The "gap size" is basically the "limit" between; does the cutter 'stay down' when moving to the next cut path, or does it retract. 'Gap' in a nutshell; "Does the tool stay down, or does it retract"?

There are times where you want the retracts, and other times you don't. Changing the Gap Size gives you control over this behavior. 

[cncappsjames]

19 hours ago, Colin Gilchrist said:

I've heard people asking "why even have both a Tool and Construction Plane? Just make it one, and it would be less confusing".

aaaaaaaaaaaaaand, Mastercam would then be less powerful for us users that like to TELL our software what to do instead of asking it to do stuff for us.  Those are probably the same people that have no idea why you would want to turn off gouge checking.

[Colin Gilchrist]

5 hours ago, cncappsjames said:

aaaaaaaaaaaaaand, Mastercam would then be less powerful for us users that like to TELL our software what to do instead of asking it to do stuff for us.  Those are probably the same people that have no idea why you would want to turn off gouge checking.

There are so many powerful features inside Mastercam, that most programmers have never touched, or even knew existed. Take (as you know very well James), the Canned Text Function. Used to trigger up to 200 different "events". These are usually a single M-Code, but a good Post Developer can do much more than that.

For example; any Canned Text number, between 5-200, will output "that number with a capital M in front". Need to output M114? M178? Just make sure the Post Text (through the CD), has that Canned Text Number enabled.

With "Miscellaneous Values", (10 Integers, 10 Decimal Numbers), you can pass data (switches and values) to the Post, to trigger output based on logic in the Post (that you write). This only occurs at the Tool Change Event though. That is important to understand. 

With Canned Text, there are 200 triggers, (integers 1-200)  and the event can be output "before", "with", or "after" the Tool Change Event. Exactly where this before, with, and after code is output, can be edited by the Post Developer. 

But something even better is that you can use either Change at Point, or the Toolpath Editor, to trigger a Canned Text Event to output code, anywhere inside the Toolpath Motion code.

> Insert M00 or M01 events, to change clamps, in the middle of the Toolpath. But also > output code to restart the spindle and coolant. This requires editing the Post though.

> Output a full Subroutine or Macro call statement anywhere.

> Trigger output of Variable Capture from Probing routines, after the Probe Point (custom drill cycle)

> Output (Custom Comments) before/after M-Codes. (CHANGE CLAMPS), (FLIP STOCK), (ADJUST COOLANT LINES), Etc.