Reverse Depth Cuts: How do you pull this off now?

[huskermcdoogle]

Long time no see folks, been buried under a pile of work, almost none of which has been programming related. I took a new job with a large company a while back and it took a while to get Mastercam purchased get posts developed (still working on that), and have time to whip up some test programs. All of my coding has been done by hand here to date, and it is time to start using CAM to optimize for tool life and reliability for some operations, as well as confidence that I don't have any stupid errors omitting features or some such issue.

 

Anyway, I have a back facing operation that I have to prove out that requires a 10" slotting saw at a 12" projection. I have to work from the Z- to the Z+ with shallow depth cuts. I have played around trying to get it to do it, but can't for the life of me get it to work leading me to believe it can't be done in a conventional manner. I swear i did this before, but maybe it was a ramp which I know can be done. So to get around this for now I have just chained my paths at each depth and used an incremental value of zero to control the depth, but making changes to the depth cuts is slow and cumbersome and requires me to move and add chains as needed.

 

Anyone have a faster way?

 

Husker

 

 

Currently Running X6 MU2 Mill Level 2

[MoMo1108]

do you have a sample or pic from snipping tool .... sounds like paralle z would be best but im not sure what your doing

[gms1]

Without pics I am thinking a thread mill cycle or a straight up point to point program.

[huskermcdoogle]

Can't snip anything from the part, but picture facing something from the back with your depth cuts working from the bottom up. But say you would do it by entering values like below

[MoMo1108]

try paralle z if you have multi axes with your key cutter

[RayD]

If your profile is a circle (backbore from the sounds of it?) Threadmill toolpath is usefull for more than just threads.

[pip]

Try toolpath transform, and delta 3d.

[pip]

 

This will produce 10 cuts incrementing upwards at 0.1mm

[huskermcdoogle]

This is my tool path using my many chain pita method. Tool path is ordered bottom up. Can't use thread mill because I can't ramp with that cutter, I have a feeling it would do bad things...

 

Cutter enters on center and then leads into cut goes around then leads out changes depth up and repeats.

 

[RayD]

Surface finish Flowline would do that, just pick your Bottom edge for step direction

[huskermcdoogle]

What would you use for geometry?

[djstedman]

Looks like pips suggestion would work great just chain the lowest geometry and the use a transform toolpath on it..

[Colin Gilchrist]

For flowline, you would need to take your chain, translate it up to the top cut depth (+ the thickness of the tool), and then use those chains to generate a surface.

 

Surface Finish Contour would also work. It has a control to order cuts bottom to top.

[Aaron Eberhard]

And if you don't feel like making a surface, you should be able to do the same with the WireFrame : Lofted toolpath, but you'd have to draw your own lead-in/lead-outs... Just make the bottom shape and then the top shape, and select them in that order.

 

Personally, I'd make a surface

[Chris Rizzo]

Surface Finish Contour would also work.

 

 

Surf fin contour is very nice because you have all the lead-in/out controls. Also work with your filter setting and you can get some nice arc motion on the whole thing.

[pip]

can you use tool offsets in the machine to allow for tool wear, with surface machining.

[Guess_who]

I know this is an old thread, but I was just going to ask the same thing. Seems like a very simple improvement that MasterCam could do with a simple toggle "cut bottom to top" or something like that.

 

I would love to see something like this added.

[Sticky]

Just ran into the same problem a couple times on a part I am doing right now with some O ring glands on a boss, and using a key cutter to undercut a boss. I did a translate to get it to work like pip's suggestion. But count me in for wanting a "cut bottom up" option on depth cuts.

[Matthew Hajicek - Singularity]

Send it to QC as a feature request.

[Sticky]

Just sent off the request, with a nice description, link to this thread, and 5 screen shots of the backplot and setup I am using to get by now.

[crazy^millman]

Sticky, I have been using Dynamic Contour for my grooves and such and have great results on surfaces finish and tool wear as well.

 

The surface finish contour does give the option to feed from bottom up, just make sure you go in the advanced settings and use the only selected surfaces to get it to stay inside the area you are machining. I will also use the Entry/Exit arc/line with High Speed setting the Loop Length and Ramp Length to get a smooth entry and exit.

 

HTH

[Sticky]

Dynamic contour will give finishing like accuracy?

 

I only have level 1 so I am limited to the more simple tool paths.

[crazy^millman]

Dynamic contour will give finishing like accuracy?

 

I only have level 1 so I am limited to the more simple tool paths.

 

Well I am doing straight on square wall grooves along with o-ring grooves that I can cut to size with a too size tool it works very well also. Problem with contour is the lead in and lead out along with the overloading of the tool. The Dynamic contour does almost like a spiral.

 

Level 1 is really limiting your ability to use Mastercam in my humble opinion. Not sure the type of work you are doing, but Level 1 will get the job done. Reading some of your posting Level 3 I think would changed some of your ideas about how to do things and would make your life a lot easier. Shoot me one of your more complex parts and I will be glad to see if I can point out some things Level 3 will allow you do to better and faster.

[Sticky]

Well I am doing straight on square wall grooves along with o-ring grooves that I can cut to size with a too size tool it works very well also. Problem with contour is the lead in and lead out along with the overloading of the tool. The Dynamic contour does almost like a spiral.

 

Level 1 is really limiting your ability to use Mastercam in my humble opinion. Not sure the type of work you are doing, but Level 1 will get the job done. Reading some of your posting Level 3 I think would changed some of your ideas about how to do things and would make your life a lot easier. Shoot me one of your more complex parts and I will be glad to see if I can point out some things Level 3 will allow you do to better and faster.

 

I'm open to doing that.

 

I don't do any surfacing, which is why I've never really given much consideration.

 

What I do is HMC work. Mostly lots of small parts, machined from solid or castings, with multiple planes. Lots of in process inspection. Most of the features themselves are fairly simple. Its the tolerances and materials they are machined from that make them more tricky, along with trying to hit the required production pricing and necessary cycle times for them.

 

The only thing I have seen where maybe level 3 could be an advantage is some of the under cutting I do. I chamfer EVERYTHING in the machine. So I use a lot of double angle chamfer tools, lolipop mills etc for deburring through and cross holes, T slots, O ring glands etc.

[crazy^millman]

I'm open to doing that.

 

I don't do any surfacing, which is why I've never really given much consideration.

 

What I do is HMC work. Mostly lots of small parts, machined from solid or castings, with multiple planes. Lots of in process inspection. Most of the features themselves are fairly simple. Its the tolerances and materials they are machined from that make them more tricky, along with trying to hit the required production pricing and necessary cycle times for them.

 

The only thing I have seen where maybe level 3 could be an advantage is some of the under cutting I do. I chamfer EVERYTHING in the machine. So I use a lot of double angle chamfer tools, lolipop mills etc for deburring through and cross holes, T slots, O ring glands etc.

 

The machining from Billet using the HST toolpaths and some of the toolpath options talked about here is what the level 3 would help you with. When I am doing Manifolds I do a lot of the same things. Just a process of doing what we can to get it done and get it done the fastest way possible.