Spherical Bore Milling

[paulfell]

The screenshot shows a Spherical Bore - we machine various similar parts with difference size bores. These parts are programmed using Mastercam for everything apart from the bore, to do this we insert a pgm to finish bore, which is editable to hold exact size of the bore, we use a Heidenhahn pgm using variable q values ( similar to # values on Fanuc), we use a depo cutter (similar to Lollipop Cutter). This works well and is fully adjustable. Is there a way in Mastercam to machine a spherical bore, with some control over the size ( i.e. Cutter Comp ) . I know i could just repost and run with different stock allowance to adjust size - but this requires a programmer to be on hand when job is running - rather than an operator adjusting it at machine, I dont think there is a way - but thought i would ask 

[Matthew Hajicek - Singularity]

You could do a flowline, make sure all the moves are one-way, and manually add your G41 or G42.  Make sure you have a lead-in and lead-out move.  I've done this once or twice.

[crazy^millman]

I think you could control a diameter, but a spherical shape is not just a diameter. There is a lot that goes into cutting a spherical shape than just holding a size. Would like to see the marco the machine is using as I have to assume it is a little more than just adjusting one pgm to allow it to maintain the size of the spherical shape. There has to be something to define the spherical shape diameter. The land of the Spherical shape and the diameter of the tool cutting the shape. Are you using a probe on the machine to check the size or are they using an air-gauge to check the size?

[Colin Gilchrist]

Sure... but some of the needed code isn't necessarily "out of the box".

 

Machining the surface could be done with either Flowline or Surface Finish Contour. You can use the "direction" button for surface lead in/out. You need to disable the gouge checks to get undercut output.

 

For 3D comp, you run the 3D Comp Chook. This converts you 3X NCI data into 5X NCI data format, that contains a Surface Normal Vector, in addition to the tool tip position. You'll need to modify you post to output the 3D comp "on" command. And you'll need to modify the 'plinout' to output the vector data. The machine will use this info to compensate in the vector direction, which is based on each individual tool position. What options does your control support for 3D comp?

[jlw™]

You can actually do this easily with 2d contour. It takes some work and a shiznit ton of clicking but it can be done and post ready inside of mastercam. Easily too. We run control so this is it, if you run wear it's easier.

 

 

1. create a surface offset the radius of the tool you want to run bigger than your drive surface.

 

2. Use surf fin contour or flowline on the offset surface and backplot then save the geo to level.

 

3. go to the geo level and delete all rapid, clearance and other stuff you don't want.

 

4. run a 2d contour path chaining all the geo you just cleaned up and set everything linking to incremental except clearance. make sure you got lead in/out so that you don't gouge the shazzer out of your part.

 

 

5. enjoy letting your guys sneak up on it and not reposting.

 

 

 

I don't have any now at this job but if you can send me a file I'd be glad to smack a path on there to show you.

[paulfell]

macro we use rotates around a circle centre in Y & Z (in 1 degree increments) allowing for rad of tip - then changes circle centre to X & Y and mills 360 degrees - changes back to circle centre in Y & Z iand repeats process - so theory is good - we just work to a go/nogo ball - not sure what an air gauge is? .

 

Not familiar with 3D Comp Chook - will investigate more - what do you mean by options for 3D comp ?

[Colin Gilchrist]

Normal Cutter Compensation is 2D (G41/G42). That works great for a Contour, but not so great for a true 3D surface.

 

Haas for example, has G141, which is 3D comp. The compensation value is "spherical", so you can compensate a 3D surface. This would allow you to use a reground ball endmill for example, and still cut the same resulting geometry by applying 3D comp.

[paulfell]

no 3d comp on control - I will give the geometry off surfaces 2d contour method a go - still trying to workout if the theory is correct - but will give it a go

[crazy^millman]

Been years since wrote one, but I think I could write a macro to do this that Mastercam can fill in the blanks using a custom drill cycle. Math is pretty basic math just need to decide on a few form factors to define the variable and the loops and would be good from there. Mhoppe or cncchipmaker come to mind as two that could probably write and very neat macro to do this.

[taperlength]

You could post several subs, each with different stock allowance and the operator would just change the sub call in the main program to make the sphere bigger or smaller.

[paulfell]

I am trying contour method suggested - ok in theory - but tool is 16MM dia, and smallest part of sphere is 17.3mm dia. so not much room to get tool in and out - at the moment tool would damage bore as it retracts , and even though the lead in is adequate at top at bottom of bore - once machining centre - it hits smaller part of sphere as it retracts - I need to either stop it retracting or keep it on centre as it retracts - any ideas ? see pic for op and some settings

[Colin Gilchrist]

Use Circle Mill - Start at center

[paulfell]

Never used Circle Mill before - once i'd found the setting to start on centre - that did it - thanks - does circle mill have any other advantages over contour ?

[Colin Gilchrist]

Well, yes, but it also has some limitations as well. For starters, it is only for "points" or "Arcs". So you're limited to only cutting "holes" with it. But it does have some great options for "Rouging", including allowing you to use a Helical Entry, and then allowing you to control the stepover, giving you some "High speed" capability to rough the hole. You can do Rough passes, semi-finish passes, and finish passes with the same path. You can choose your lead in/out options to start at the center, and use "perpendicular" entry if you need to turn on cutter compensation.

 

When machining Arcs, you can choose multiple arcs, of different sizes and depths, and the path will adjust accordingly. If you choose "points", those points become the center of the circle, but you get an option inside the tool path to enter a "diameter" for the arc you are cutting.

 

If I'm milling holes, or counter bores, I prefer Circle Mill to do that.

 

Technically, if you are chaining with Contour, you can "chain a point" before and after the circular chain, and use the "start at point" and "end at point" options in the Contour Lead In/Out, but that's a bunch of extra work considering you always want to start/end in the center of the hole. Circle Mill does this nicely.

 

Since you are chaining multiple arcs, I'd set the "Top of stock", "Depth", and "Retract" values to 0.0 Incremental. That will allow you to add each arc in succession in a single tool path, and not have the tool retract between each chain. Then I'd use the "Approach" and "Retract" Points to give my tool the plunge and retract from above the hole. That will give you a single "plunge" point at the beginning of the path, then your tool will cut each chain (feeding from/back to center), and finally the "retract" point will pull your tool out of the hole for clearance...

[civiceg]

"You could post several subs, each with different stock allowance and the operator would just change the sub call in the main program to make the sphere bigger or smaller."

 

Have it tied into the diameter comp via macro. 

[jlw™]

Use 2d contour, put a point in the middle then click the check box on lead in/out by use entry/exit point.  Boom.

[jlw™]

[paulfell]

Thanks - I didnt know about chaining a point either - like the look of circle mill - very useful info- thanks

[jlw™]

2D contour is a lot more useful than people realize. You can also cut tapers/cones with it with cc. I still old school stuff with it when I can't get exactly what I want out of area mill then trim it to shape to minimize machining air.

[Matthew Hajicek - Singularity]

A wireframe toolpath might serve well too.

[jlw™]

Can you run cc on any wireframe paths?

[Colin Gilchrist]

Hmm. I don't think you can compensate the Wire frame paths. For 3D compensation, I've always used the full surface paths like Flowline, and used the 3D Comp Chook. Take the example of machining a true Hemisphere. In order to adjust the spherical shape, 2D contours wouldn't accurately compensate, the closer you get to the bottom of the Hemisphere. To truly compensate the shape and maintain the geometric form, each tool position needs a normal vector at the contact point. At the very bottom, the compensation vector would be completely Vertical, but at the equator, each vector at the contact point would point in XY towards the center of the sphere. That is true and accurate 3D compensation, and your control must have an option in the Gcode to enable and disable the 3D comp.

[jlw™]

Totally agree Colin! Definitely a potential for error if comped too much. However, in his case he's talking tenths or worst case thousandths so the error would most likely be impercievable.

 

I will look for this chook tomorrow. I had no idea.

[Colin Gilchrist]

I agree fully on this application. The error would most likely be less than the resolution of the machine (it might approach .0001) at the upper and lower limits of this particular shape. Especially since the tool itself is so close to the size of the sphere being produced.

 

Comp 3D does require modifications to your post to get the proper output. It is not OOTB in any way. You need to detect that the NCI Gcode is '11', and add some code to output the Comp Vector (usually IJK parameters) along with the XYZ position of the tool tip. The IJK is a unitized vector that is normal to the point of contact of the ball sphere in contact with the compensation surface.

[Matthew Hajicek - Singularity]

Can you run cc on any wireframe paths?

 

Not as posted; you'd have to add it manually.  I suggest it because the code would be smooth and precise, so the comp would apply well.  Sometimes surface paths have little squiggles that throw comp for a loop.