Why is boring on the Lathe so difficult

[Rocketmachinist]

I am trying to bore 1.125" strait bore to a flat bottom. I have drilled with a .500 drill and now trying to send an E06STLPR2 boring bar with a TPGM21505 insert into the hole and bring it up to size. What am I doing wrong. What chain do I have to select (The strait chain, the strait chain and the bottom?) . How do I tell the tool the minimum size I want it to start boring at. DO I have stock recognition on?

 

Please help, and thank you in advance.

[uncle_dolan]

Hi Rocket,

 

for a quick fix you could try creating a finish toolpath along the straight bore, and just tell it how many passes at a specified depth you want it to do.

 

Alternatively you can seelect the whole contour of the bore and shorten the exit line in your lead in/out paramaters to stop it from cutting too close to the centerline.

 

Hope this helps!

[Rocketmachinist]

Also, why can I not get threading inserts to match up with "grooving bars" I found a E08-NER2 under the grooving tool library but that means i cannot select a NTP2L insert so I can thread with it?

[crazy^millman]

Rocket that is about one of the easiest things you can do. What kind of errors are you seeing.

 

On the threading make your own tool export grooving tool to a level and the threading tool to a level and make your own tool.

[Rocketmachinist]

What was happening was boring rough was recognizing the drill point angle and wanted to clean it up even though the tool cannot handle a bore that small without crashing. I was playing around with stock definitions and other such things to tell the tool where to start. I ended up having to rough the bore with 1 finish pass telling it how many passes to take and then take a second finish pass with the bottom taken into effect so I can do a clean up pass.

 

I also really don't quite get why you can only use look up tool and inserts that are used for a specific operation. That just seems soo counter intuitive to me. They need to make the holders for Top-notch inserts available for both grooving and threading. :wallbash:

[uncle_dolan]

I dont use the tooling libraries that are built into mastercam lathe. We dont do a great deal of lathe work and we will generally use a range of say 20 tools to machine MOST jobs. This being the case I just went through and made my own tools / library and have never had a problem with tool definitions. For a lot of the tools i just use the standard holders as a base and just modify them without the need to redraw entirely. It doesnt take too long to set up, and once it is, life is alot easier!

[K2csq7]

There are sooooo many PITA things about lathe....

I draw at least 70% of my tooling and, for the cuts, I draw geo & chain it. Never use lead in/out, always use lathe finish.

I am with Brendan, we only really use a package of a couple dozen tools, the rest are custom anyway... Even modifying tools from the library gives me headaches.

[DavidSV]

If you want it to know where to start roughing, use stock.

 

The MC Lathe is not that hard, but I think most people are "Mill People" and just don't know what is going on. When I started programming the lathe, I was a mill guy that got thrown in because our lathe guy quit. I had to go to my reseller and get a crash course on the lathe and then start trying to program with it. Our "Lathe Guy" didn't use MC, and instead used some antiquated software from he 80's that we had to have a special super old computer to run. After I got a decent post and a little trial and error, I was programming some pretty cool lathe parts. Its pretty easy to use, but you can't program it like the mill.

 

Oh, and just post the roughing long hand, not canned.

 

So, to bore the hole. Assign stock so the software knows what its tying to cut.

 

Drill the hole. Run an end mill into the hole to make it flat bottom leaving .001-.002 for cleanup.

 

Draw the ID and back of the hole. Break the line at the back of the hole at the drill size. Chain the ID and back of the hole down to the drill size for roughing. Use the stock for the stock. Make sure you leave some stock in X & Z for cleanup. Chain the finish pass to the center.

[BBprecise]

Hi Rocket,

 

for a quick fix you could try creating a finish toolpath along the straight bore, and just tell it how many passes at a specified depth you want it to do.

 

Alternatively you can seelect the whole contour of the bore and shorten the exit line in your lead in/out paramaters to stop it from cutting too close to the centerline.

 

Hope this helps!

 

Do Brendans second suggestion, go to lead out page, click to enable "Adjust geometry" and then shorten up the geometry by 1/4" (assuming you have the bottom of the bore drawn to X0, remember MC works radially on lathe dia's so 1/4" radially is 1/2" dia). I prg. equal amounts of milling and turning so lead in/out options have become my friends .

 

On another note, why not just drill the hole bigger? We use Ingersolls Quad Drills and they leave a fairly flat bottom, but even a bigger HSS drill (assuming that's what you're using) would make things easier.

 

My 2 cents.

[heavychevy2155]

One thing I would do when using Lathe, I would change my drill point angle to 175 degree's and it wouldn't make the boring bar want to start at the minimum bore dia. I haven't ran lathe for years but I have to say, I got pretty good with it and could make it do almost anything I needed. It took alot of trial and error but I finally figured out the best way to get good code and I would pretty much just post and go. I ran V9 lathe so it's been years to say the least.

[Rocketmachinist]

I ended up taking Brendan's suggestion and chaining the main bore and the back wall and then shortening the contour by .250. It seems to work pretty well now. I just have to learn all the workarounds I guess.

[Colin Gilchrist]

We've recently had a discussion about how to improve boring in Lathe. It was suggested that we think about creating a specific "Boring" toolpath that would have more intelligence. Thanks for the feedback, I'll run the suggestions up the chain...