MC Lathe canned cycle comment

[PE @ IHS]

Hello everyone

 

As folks with lathe experience know, there are 2 versions of the G71 rough turning cycle available on Fanuc controls (similar on Haas, Okuma, etc.) One format (Type I) only allows no undercuts, while Type II allows undercut geometry. It seems that MC doesn't differentiate between the two, the main difference being the necessary addition of a Z rapid command in the first line of the profile definition call

i.e.

...(TYPE 1)

G71 U.1 R.01

G71 P12 Q13 U.02 W.01 F.01

N12 G0X1.

G1Z-.5X1.22

X1.4

Z-2.

N13X2.

...

 

...(TYPE 2)

G71 U.1 R.01

G71 P12 Q13 W.01 F.01

N12 G0 X1. Z.005 (z call to acivate Type II)

G1Z-.5X1.22

X1.4

Z-2.

X1.25 Z-2.38 (undercut)

N13 X2

...

 

does anyone know if there is a way to differentiate between these two cycles in MC (since canned cycles in MC do not seem to have plunge parameters available)

 

thanks

 

Peter Eigler

[Glenn Bouman]

Are you refering to this post switch?

 

old_new_sw : 1 #Switch old (6T), new (0T+) cycle formats, 0=old, 1=new

[PE @ IHS]

Nope, as far as I know this switch toggles between single line and 2 line canned cycle formats.

 

i.e Fanuc 3T, 6T, 10T

G71 P20 Q30 U.02 W.01 D.1 F.008 (one line)

 

********************************************

Fanuc 0T, 18T, 21T

 

G71 U.1 R.02

G71 P20 Q30 U.02 W.01 F.008 (2 lines)

 

[ 10-02-2002, 08:21 AM: Message edited by: Peter E ]

[jeff]

Peter,

The plunge parameters tab in on the lower right side in the rough parameters window.

[gstephens]

You have to compare x coordinates throughout the whole chain (really tough to do), and determine whether or not the x value gets smaller then larger over the course of the cut. Somebaod has probably done this for a post at some time (Yasnac?), but since the canned cycle code changed with v8, I'm not sure if anyone has dealt with it since. I'd look into it myself, but I'm swamped at the moment.

[PE @ IHS]

after some checking, it appears that MC only supports the type I canned cycle (no undercuts will be supported in the code, though backplot APPEARS correct)

 

thanks for the replies

 

Peter Eigler

[McRae]

Peter,

 

Are you an advocate of Canned Cycle Output?? I am of two camps depending on the type of shop that I am at. If quick changes are needed to adjust DOC right at the machine etc, then the canned cycle approach is what you want. For the more elegant approach, I would stick with the line by line execution as the Canned Cycle really doesn't have an elegant re-start sequence.

 

Secondly, lets think a minute about tooling. For using undercuts, a weaker edge (MDJNR or Equivalent) would be neccessary and this would defeat the purpose of using a "Roughing" operation which is get the material off fast!

 

[Webmaster - Removed the somewhat incendiary comments in order to keep the peace. Behave children.]

 

[ 10-06-2002, 11:39 AM: Message edited by: Webmaster ]

[PE @ IHS]

Hi Andrew

 

People running machines generally prefer canned cycles, since it gives them more control. Shop owners who program manually and are considering buying Mastercam need to see code during their demo that they can relate to (subprograms, canned cycles etc.), instead of many extra lines of code. Non ferrous metals as well as many steels can easily be roughed with DNMG or DCMT inserts and it makes sense to use the same tool for undercuts such as thread relief grooves than to waste time indexing to a grooving tool. Canned cycles are great when programmed properly.

 

Aluminum, brass, and copper are actually better roughed with 55 deg tools, since the long stringy chips are less likely to get wedged at the back of the insert and rub along the part.

 

Peter Eigler

[McRae]

Peter,

 

Great post, that is correct that people will be more receptive to the system if it will produce the same format as to what they are used to. The job of the software however isn't just to show how it is, but how it could be!

 

Having served my time in the sweat shops of hell, I must admit, the canned cycles were much easier to manually program... The use of offline programming takes the apparent power away from the set-up/programmer/machinist guy and places it squarly in the hands of the programmer (where I think it belongs). I avoid using the canned cycles (in turning) so I can maintain control of the process and keep the errors caused by our "Operator/Machinists" out of the equation. I create enough problems already on my own... Perhaps this could be an additional benefit that the prospect wasn't aware of. Ask him/her how many times that they had a great setup only to have the night shift slow the thing down!

 

Hope this helps and gives you a second opinion for the bag of tricks.

 

(Sorry Webby for the previous post snippets... Jack is still on vacation anyway!)

[gstephens]

Update:

 

coming in a future (probably not v9.1) release of Mastercam lathe...Plunge parameters in canned cycles and the ability to extract the setting from 10000 parameters (for those of you who understand ) in the post.

 

It's still going to be a pain for Yasnacs that need to know "how many valleys are in the chain".

[Michael Reynolds]

Peter,

 

With all due respect (and I mean that), I've seen programs come down from, well, programming, that have HAD to be fixed by the "operator". Sometimes thats what keeps the floor running while the programmers are not there.

 

Converesly, I've seen your point too, when no matter what operator is running the job, they HAVE to "fix" it.

 

Both sides, now...

It ain't a perfect world our there...

 

Respectfully,

 

Mike R.