Is this an MC Lathe problem?

[g-codeguy]

Simple part. Want to rough turn including rear OD chamfer. Lathe Rough Toolpath won't work. Have to select Lathe Finish Toolpath. Why? Is it a Mastercam problem? Or are my settings wrong? Settings are as downloaded. I've made only minor changes per reseller & hints from the fine gentlemen on this forum. Most changes I made were to the posts.

 

I think this may be why I had the problem mentioned in the earlier thread I made today. I had used the Rough Toolpath.

[Guest]

DO you have stock defined?

 

Biggest issue I see continually.

 

BTW, it sounds like a training class at your resellers might be in order as well

[Goldorak]

set the correct plunge parameter in the roughing cycle

 

[g-codeguy]

Stock was defined. We had a rep in for 2 days (separated by about 3 weeks) early this year. Had him in last year for a couple days, but never got to use MC at that time because our posts weren't set up for X. We run them off a company wide server instead of off our C-drive. Couldn't get them to update to the server. That has been solved, but many of our posts are still not where they need to be. Some old ones couldn't be used in X because of their age. Wouldn't update properly.

 

You and one or two others helped me get some of them running much better, but we still don't have live tooling or subspindle posts set up right yet.

 

I admit to not using Mastercam as much as I should (or the company would like) as I prefer manual programming. Always before I would run a finish pass...leaving extra for finishing...and c/p it into my program. Remove the extra stock allowance, regenerate, and re-post it again for my finish pass. Cut-and-paste that.

 

I have been asked to do all my programming in MC. Thus I am running into problems I never had before. One thing holding us back is that we were not using X2 until this year even tho we were upgraded to X when it first came out. Post problems are one reason we didn't bother using X. Not having enough training is another reason.

 

Would you like to try this simple part, and see if the Lathe Rough toolpath works for you? .799/.785 OD, .655/.650 ID, .070/.068 thick, .015 x 45 degree typical on all 4 corners. 13/16 inch material. Rough OD leaving .005 on X and Z with 35 degree tool. Does it rough machine the rear OD chamfer for you?

 

I personally feel at the moment that this is a Mastercam problem. The other lathe programmer programs using MC only. He couldn't get it to work either when using the Lathe Rough Toolpath.

[g-codeguy]

axela: The Plunge parameters are set correctly. I always use the 2nd from left option for finishing. Had them set up that way as default in v9 to save time. Like I said before, I've done next to nothing with the X2 settings yet.

[Philcott]

G-code.

 

Try disabling stock recognition. Some times this will work.

 

Phil

[LEV]

It works here. all I had to do is extend end of contour in lead out .05"

 

Lev.

[Philcott]

the other way I do this is to go to lead out, extend the end of the contour (get used to using this it comes in handy in lots of places), then I usually add a line as well. Let's say .05 @ 180 degrees. This is with stock recognition on.

 

The issue probably has to do with your back chamfer being the same size as your/my insert rad.

 

Phil

[chris m]

Mastercam doesn't like taking less than the TNR in many cases so you need to fake it around a bit as the other guys have stated. I program both manually and with MC and agree that Mastercam is a PITA sometimes but it really pays dividends for us when we need to move a job to a different machine, make a rev change, do a similar part, etc.

 

That being said; I run V9.1SP2

[Redfire427]

Another possible cause is your tool definition. I do the operation you are trying all the time. I use a 35 degree insert and set my clearance at 2 degrees on the plunge parameters page. ( Use plunge clearance angle ). It is possible to do what you are looking for, you just must have something set incorrectly.

[g-codeguy]

Phil: Disabling stock recognition did and didn't work which I will explain in a minute. We also tried an .008R insert. Also tried a test part with .100 x 45 degree chamfers, & it still wouldn't run right. Extended contour by .05, but didn't add an extra line. Still no go.

 

Chris: See above regarding TNR. So far I like v9 better myself, but I can see that X2 has advantages. Just need to learn it like I know v9. Reason I have to do all programs in MC is because we have several makes of lathes. Powers that be want every part in MC so we only need to run a different post. I can manually modify from one machine to another faster than doing it in MC.

 

Prosin Molds: Don't see how it can be my tool definition or the 3 degree clearance angle as it runs perfect if I use Lathe Finish instead of Lathe Rough.

 

Phil, I accidently made a discovery this morning. If I eliminate the front chamfer from the geometry, Lathe Rough Toolpath with stock recognition works correctly. Add the front chamfer back in, and poop.

 

Other programmer just came to me with more information. His finding is that you can only use Lathe Rough Toolpath in one direction. Can't machine going up, turn OD, and switch direction by going back down. This reinforces what I accidentally found out this morning. Lathe Finsh Toolpath doesn't care if the tool switches directions. That is the way to go. Much less headache.

[g-codeguy]

Edit of previous post. Should say "If I eliminate the front chamfer from the geometry, Lathe Rough Toolpath with stock recognition turned off works correctly.

[heavychevy2155]

Can you use 2 roughing ops, one for front and one for rear? Then on the rear one set the lead in angle steep and use plunge parameters, then finish profile with single finish pass.

[Philcott]

G-code

 

I think you may have not used the Add Line function in lead out. When I drew up the part you described and extended the end of the contour and added the line as I described above the rough cycle worked very nicely. You weren't by chance using rough canned were you? This could be entirely different.

 

Keep trying. It does work. Also make sure your stock material is longer than you are trying to cut. Maybe make it .5 longer.

 

Phil

 

Phil

[Philcott]

quote:

---

Other programmer just came to me with more information. His finding is that you can only use Lathe Rough Toolpath in one direction. Can't machine going up, turn OD, and switch direction by going back down.

---

Don't limit your ability with Mastercam by thinking this is correct. Mastercam will most certainly rough the back side in both directions. I will try to send you a program tomorrow to show you how I do it.

 

Phil

[Goldorak]

do you need to do something like this :

 

[chris m]

quote:

---

Reason I have to do all programs in MC is because we have several makes of lathes. Powers that be want every part in MC so we only need to run a different post. I can manually modify from one machine to another faster than doing it in MC.

---

This is one of the major reasons that we use MC for turning as well. I have 1980 Mori-Seiki lathes and 2005 Okuma lathes and a variety in between, so MC works great if I need to move jobs around. I can create a program for a different machine in seconds using MC and know that it is correct, where manual editing requires a lot more concentration and time to get this done. When I first started using MC at V8 I would get VERY frustrated because I had many an episode of fighting with the software to machine a simple feature like the one you're doing; It would take an hour to make a finish toolpath when I could've programmed the whole job in 15 minutes. Now that I have the workarounds and little glitch fixes burned into my brain, I am at least as productive with MC as I was with the pad of paper and pencil. MC has also eliminated all of the typos and screwups that had our guys single-blocking every program the first time through and I think it is well worth the time investment; I know it sucks now but you'll be glad when you have it mastered.

 

C

[g-codeguy]

Heavychevy: No problem doing it with 2 ops, but that is not what I want.

 

Phil: Am not using a canned cycle for one pass. I did not use the Add line function before tho I did extend the line by .007. I've done it before, but don't know how to accurately do that with this part so I extended the geometry the desired amount, put an arc tangent at the end point (size of tool radius), created a 90 deg. tangent line, trimmed the vertical and 45 degree line, rechained geometry to include the new lines. It machined the rear chamfer, but not in one shot. I can accomplish the same thing without adding the line. See program example.

 

Stock was defined to include 5 parts plus a little extra.

 

axela: That is basically what I want except my chamfer is small enough to be done in one shot. See comments to Phil.

 

This is the output I am looking for, and can get with Lathe Finish Toolpath (minus the F.008):

 

X.7134Z.02

G1X.798Z-.0223F.005

Z-.0787

X.7458Z-.1048F.002

X.82F.008

 

 

This is what I get with the Lathe Rough Toolpath:

 

X.7141Z.0208

G1Z.0196F.005

X.798Z-.0223

Z-.0787

X.7978Z-.1048F.002

X.872F.005

G0X.922

Z-.0787

X.798

G1X.7458Z-.1048F.002

X.82F.005

 

 

End result is the same, but 11 blocks vs. 5 blocks. Not nearly as pretty either!

[Philcott]

G-code,

 

One important skill to learn when useing a cam system is (once you have your post dialed in) to stop reading the code. It has taken me a while to stop fretting about how many lines of code I get when posted with mastercam but I now don't care. What is important is how it cuts the part.

 

If you increase your roughing depth of cut that "may" take the u-cut in one pass but I'm not sure.

 

good luck.

 

Phil

[Goldorak]

i got to be agree with phil

 

don't waste your time to get the cleanest g-code possible

 

if it's work and the machine memory can handle it , leave it like that

[g-codeguy]

quote:

--------------------------------------------------------------------------------

This is one of the major reasons that we use MC for turning as well. I have 1980 Mori-Seiki lathes and 2005 Okuma lathes and a variety in between, so MC works great if I need to move jobs around. I can create a program for a different machine in seconds using MC and know that it is correct, where manual editing requires a lot more concentration and time to get this done. When I first started using MC at V8 I would get VERY frustrated because I had many an episode of fighting with the software to machine a simple feature like the one you're doing; It would take an hour to make a finish toolpath when I could've programmed the whole job in 15 minutes. Now that I have the workarounds and little glitch fixes burned into my brain, I am at least as productive with MC as I was with the pad of paper and pencil. MC has also eliminated all of the typos and screwups that had our guys single-blocking every program the first time through and I think it is well worth the time investment; I know it sucks now but you'll be glad when you have it mastered.

--------------------------------------------------------------------------------

 

 

Yeah, I make the occasional typo. Refuse to admit how often. We have one Okuma, but I am not the one programming for it unless the other programmer is on vacation. I couldn't manually modify to the Okuma from our other lathes faster than using MC. Canned cycles in particular are too different. Nor do I normally program for the EMAGs which also require a lot of changes.

 

However, much of my program changes are between Hardinge lathes and Daewoo lathes of various models or between lathes of the same make but different models that might require minor changes. All use Fanuc controls. I have macros set up in the editor. Click on the macro icon, click on the desired change, click ok. No typing. Very fast.

 

I do like the fact that I don't have to worry about typos causing a crash, or alarming because I missed a code or something.

 

I like my programs to be as clean as possible. I can get very close with MC, but it takes a lot longer to achieve. We make a lot of studs for a sister company. Almost all have at least one under-cut at a shoulder. These in particular require lots of modifying, regenerating, re-posting, remodifying, regenerating, re-posting, etc. since I rough these out for the same reason I rough .015 x 45 degree or larger back chamfers as in the part we have been discussing. That is because most times the finish looks like crap if I don't.

[g-codeguy]

Phil & axela, you posted while I was typing up my reply. I have to admit that your remarks are probably right on. Awful hard for me, tho, to break old habits. Those habits are probably why X2 is still giving me fits at times.

 

I do appreciate all the help I have been getting. This is the first place I turn to for any questions on MC. Even before emailing our reseller. Usually get a quicker answer, too!

[Philcott]

G-code,

 

I've been in this game for a long time and was one who was always pretty anal about how my program looked. "X" had to come before "Z" which came before an "F" and so on. It has been hard for me too to let that go.

 

Have you ever tried to save an operation file? If you have a process that works well for you in regards to speeds, feeds, tools, depth of cuts, etc you can save them and call them up into a new mastercam file and all you need to do is pick the new geometry to be associated with each operation, regenerate it and voila your done.

 

This can be a big time saver on family of parts.

 

Phil

[g-codeguy]

Phil, no I haven't. Wouldn't know how to start. Could you give me a little more detail on how to do it?

 

And, yes, I am also pretty anal about how my programs look.

 

Did some part-time programming for another company. Their programmer could only use MC. He didn't know how to manually program. The set-up guy told me he much preferred my programs. They were much easier to follow.

[Philcott]

I'm off for a three day weekend music festival so I'll get back to this on Monday.

 

Earl Scruggs, Taj Mahal and others. Beer, pickin' and grinin', sunshine, floating down crystal clear rivers, good food and best of all girls dancing all around me with their inhibitions cast into the wind.

 

"Excuse me can you rub some sunscreen on my back? .... Thank you."

 

"No, Thank you."

 

Is life good or what?

 

Phil