Plunge Milling in Mastercam

[FROZEN]

Monkey Meters

[jlw™]

Well I finally figured this shït out.

 

Plunge does NOT like WCS and it really doesn't like a T/C plane from a WCS.

 

But you can trick that mutherfocker.

 

You gotta ignore that zigzag shït and use nci from a 2d contour path. Set the geo for the 2d path completely z negative of the drive surface. Then create your plunge path to the best you can, green check and let it generate. Now change back to Top/Top/Top and open the parameters back up, go to cut depths, use absolute and pick the points relative to Top/Top/Top even if you are in a tilted plane. Now, regen the nci path and then regen the plunge path and it will give you proper clearance, retract and feed planes as well as respect the drive surface.

 

So far, all output has been good.

 

Really glad I fingered that out, I've got my dang Iscar Tang Plunge up to 24 cubes in 4140. Everybody is asking if I'm gonna givem the tang. I say "of course, you know I love tang!"

[BrianP.]

37/64ths FTW!!!

 

Hey you started it.

 

"The system of imperial units or the imperial system (also known as British Imperial^[1] or Exchequer Standards of 1825) is the system of units first defined in the British Weights and Measures Act of 1824, which was later refined and reduced."

 

Oh wait. That's right your French.

[mkd]

Is there a software package out there that will drill down to a very curvy surface from a grid of circles/points that denotes exact drill locations? Thinking NX or catia might do it.

[Guest]

3 minutes ago, mkd said:

Is there a software package out there that will drill down to a very curvy surface from a grid of circles/points that denotes exact drill locations? Thinking NX or catia might do it.

Mastercam can do it......

https://www.dropbox.com/s/wdj4pe2432gzfod/PLUNGE MILLING SAMPLES.mcx-9?dl=0

[mkd]

I messed with grid but the spacing does it's own thing as far as positions.

 how do you control the EXACT positions with NCI method? USing drilling for plunge and project doesn't produce any motion/ errors out.

[jlw™]

I've messed with plunge milling A LOT since this post.  I've learned a good bit about applying it.  Can you share a file?  I can probably throw a few paths on that will help you out.

Also, WCS really, no REALLY, messes with the surface plunge path.

[huskermcdoogle]

On 9/13/2016 at 1:35 PM, Colin Gilchrist said:

But, there is a new feature available. In the ModuleWorks paths, they have a Plunge option. And they allow you to move off the wall before retracting! So I'd recommend using the "triangular mesh" paths and using the Plunge option.

Where is this?   Tried to find it and don't see it as an option in the Tmesh toolpath.

[mkd]

I guess the best option would be create lots of geometry points and a good old drill cycle to incremental depths.

As far as creating points, perhaps extruding the circle down to the crazy-part-surface and creating an intersecting curve will help get drill depth points.

[Matthew Hajicek - Singularity]

Will it pull the cutter away from the work at the bottom of the stroke before retracting?

[crazy^millman]

I would create my line and then my pull away. I would then do a 3D Contour using that and away I went. More work, but I can always put the tool where I need it and always pull it off like I want every time. Other ways to do it, but I got out of Plunge Milling sometime ago.

[Colin Gilchrist]

I haven't looked in the options for plunge since X9. Not sure which paths it is available in anymore...

[huskermcdoogle]

19 minutes ago, C^Millman said:

Other ways to do it, but I got out of Plunge Milling sometime ago.

I am guessing now that there are decent multi axis adaptive strategies, that is the route you went?

I think plunge milling has its place, but I think personally it would only be in long reach roughing situations, or where you need to direct the cutting forces a certain way.

Good tool to have in the chest none the less.

[crazy^millman]

3 minutes ago, huskermcdoogle said:

I am guessing now that there are decent multi axis adaptive strategies, that is the route you went?

I think plunge milling has its place, but I think personally it would only be in long reach roughing situations, or where you need to direct the cutting forces a certain way.

Good tool to have in the chest none the less.

With 5 Axis you have a lot more freedom to rough a part than with 3 Axis. To many still stuck in the old ways to rough material. I will do whatever a customer wants, but the advantage I am seeing is the HST toolpaths with the right holders and such smoke anything else.

[Leon82]

I had one repeat job where I just drew a line with a retract attached to it sort of like a check mark and then just translated around and use a 3D chain. It was a NASCAR tang plunge and  it worked pretty good.

[Leon82]

Iscar.

[mkd]

1 hour ago, C^Millman said:

With 5 Axis you have a lot more freedom to rough a part than with 3 Axis. To many still stuck in the old ways to rough material. I will do whatever a customer wants, but the advantage I am seeing is the HST toolpaths with the right holders and such smoke anything else.

I'm looking to turn a 7 hr HSM (that has a one-way ~70% engagement time) op into a 2 hr drilling op with some indeterminate milling to cleanup added on the end.

in the very beginning stages....

[mkd]

On 9/25/2017 at 2:25 PM, mkd said:

I'm looking to turn a 7 hr HSM (that has a one-way ~70% engagement time) op into a 2 hr drilling op with some indeterminate milling to cleanup added on the end.

in the very beginning stages....

might need to pull my foot outta me mouth on this one. Just got some recommendations on speeds and feeds for drilling 6al4v and am a little underwhelmed.

120 sfm@ .003" sound ultra conservative to you, for a 3xD insert drill?

[Colin Gilchrist]

2 hours ago, mkd said:

might need to pull my foot outta me mouth on this one. Just got some recommendations on speeds and feeds for drilling 6al4v and am a little underwhelmed.

120 sfm@ .003" sound ultra conservative to you, for a 3xD insert drill?

That's really conservative. Should be more like 300-350 SFM, and .010-.015 per tooth. Depends on the particular tool though.

[crazy^millman]

MKD  was just with a customer in the last few weeks and we were running 450 sfm with 200% Doc and 5% ROC .005 Per tooth on a 7 flute and getting about 300 minutes of tool life. Almost coundn't hear the machine cutting it was such smooth cutting conditions. 

[mkd]

32 minutes ago, C^Millman said:

MKD  was just with a customer in the last few weeks and we were running 450 sfm with 200% Doc and 5% ROC .005 Per tooth on a 7 flute and getting about 300 minutes of tool life. Almost coundn't hear the machine cutting it was such smooth cutting conditions. 

Curious if you were using zig zag or one way? My customer is getting similar or slightly less life with 5 flute @350sf/m. My potential problem is that equates to throwing 3-4 endmills at the job $65+ a pop VS. a pair of $15 insert with four sides.

 My drilling idea would start with external coolant so i'd be limited to .500 or 1.00" stepdowns, i figure.

[crazy^millman]

One way, yes that is the balance of doing this type of work where is the trade off of tooling cost to machine time. If you can work it out cheaper with one process then you adopt that process if the other process cost more in tooling, but gains you machine time offsetting the tooling cost then you head in that direction. It cost money either way you go about it the trick is finding the cheaper most productive way that allows you to turn a profile making the parts you need to make.

[Colin Gilchrist]

7 hours ago, mkd said:

Curious if you were using zig zag or one way? My customer is getting similar or slightly less life with 5 flute @350sf/m. My potential problem is that equates to throwing 3-4 endmills at the job $65+ a pop VS. a pair of $15 insert with four sides.

 My drilling idea would start with external coolant so i'd be limited to .500 or 1.00" stepdowns, i figure.

3 to 4 endmills? Not sure what you mean there. How big is the part, and how much material to remove?

With the Dynamic Milling Ron is talking about above, I bet he is doing a 6-10% Stepover value.

You should be getting multiple parts per endmill. Not multiple endmills per part.

As a quick example of how I'm applying new tooling:

I took a process that was: rough with a .750 ball endmill (about .250 stock on the forging), carbide insert, at 3 IPM, then finish with a 2 Inch diameter, eight flute cobalt endmill, with a .250 Corner Radius. It took about an hour and a half to rough, and thirty minutes to finish. It used 1 ball insert and 1 finish endmill per part. The insert cost about $15 bucks, but the finish endmill was about  $300, before we had the corner radius added as a custom grind. So I'm sure the total cost of the tool was easily $400 with all the extra processing.

I replaced both tools with some new Ingersoll replaceable 5 flute tips, with .250 CR. My entry technique is basically a Feed Mill technique. I start .500 above the stock, and rotate the B Axis 18,000 degrees, while feeding Z-.48. I'm going at about 550 RPM, and 24 IPM. Then, once I've cut the 'slot' into the material, I rotate B -36,000 degrees, while moving Y -1.99. I repeat the finish paths in a similar way. Each replacement tip is about $160. But we've cut 6 parts so far with the pair of tips, and the finishing tool still feels sharp, and barely shows any wear. I bet we get another 10 parts out of the tips. Actually, I will probably cut a few more, and switch the 'finish' tip over to the rougher, and install a new finisher. But if I can get 1 tool, to cut 10 parts, we are down to a tool cost of $16 bucks a part, from over $400 before...

Do you want some guidance for your path? Can you share a part file? Don't just post it up here. PM me, and I'll share a secure folder with you.

What is the length, width, and height of the part, and how much stock are you removing?

 

[mkd]

block weighs 115 lbs and going to maybe 20lbs at this stage... so i'm figuring how to budget (if even possible)

thanks for all the suggestions on my hijack.

..and if you got a cutter that'll last 20hrs in Ti, i'm all ears $$$$

[mkd]

13 minutes ago, Colin Gilchrist said:

I took a process that was: rough with a .750 ball endmill (about .250 stock on the forging), carbide insert, at 3 IPM, then finish with a 2 Inch diameter, eight flute cobalt endmill, with a .250 Corner Radius. It took about an hour and a half to rough, and thirty minutes to finish. It used 1 ball insert and 1 finish endmill per part. The insert cost about $15 bucks, but the finish endmill was about  $300, before we had the corner radius added as a custom grind. So I'm sure the total cost of the tool was easily $400 with all the extra processing.

 

 

man that's some painful old school technique.

 

my application could actually use considerable flute length from one end, tapering shallower to the other end. A large cobalt endmill , buried, would not actually be that crazy of an approach. especially with the regrinds possible.