Thread: Semi New Mazak HCN 5000 B Axis Programming Issue

Hey Guys,

For those that don't know me, hello, I have been over on the CNC Forum for long while, though have not had any time to read, respond, or post at all for the last six months.

A few months I started a new job, and I was hoping your guys might have some advice for me with our HCN 5000 II.

I am programming using Mastercam and have run into a little snag, although it is a simple find and replace issue in the code I am wondering if it is possible to make the machine input right. I know it can be fixed in Mastercam, though would rather fix it at the machine because it would make the code cross compatible with other machines in the shop.

The problem is related to the B-Axis program inputs. Whenever I make a B-Axis move I need to program them with no decimal and add three zeros to the angle. Ex. Going to 90 degree would be programmed 90000. I have tried entering values 90. to try and get it to work like you can on some fanuc controls, but with no success. Is there a parameter that can be changed to make it so I can program will accept 90. and go to 90 degrees. Hopefully this is me being stupid, and or it is a simple fix.

If the issue isn't clear, kick me upside the head and I will rewrite it

Thank you in advance.


Husker Mcdoogle


P.S. - I am posting in the cad/cam for a little post help, most edits I have been successful with but am not having any luck changing the format for this one, once again probably a stupid problem....

I posted in your other thread...

But, I take it the machine is an NC positioner. In otherwords, its not a full rotary or true indexer? You can tell this by looking at your work offset page. If you're missing the "B" offset, then you have a 360k NC positioning table. As far as changing the display, it can probably be done but it won't do you any good since from a programming standpoint, you still have to use a "no decimal" output (what you're doing right now). So you could program B90. but the machine would only turn to .090

As for compatibility to FANUC, it should be the same. FANUC control should still read a "90000" as a 90° index as long as you don't use a decimal in the number.

What I would do? Have the machine upgraded to a full rotary. It's not that expensive and can be done in a couple days. Mechanically, the machine is already there. Mazak only needs to update the drive, small peice of software and re-set the MRJ2 for it.

Thanks for the Response.

Suspicions Confirmed...

I have been lead to believe we have a full rotary. I just looked at the offset page and there is no offset for the B-axis. So I guess that means 360K Indexer.... I am not too concerned with having to change the program output, now that I know that is what I have to do. As for upgrading I do not think I will be able to justify that to the management because we are not doing any work that would require a full fourth. Any major points I could use as justification?

Thanks again,

Husker

Husker, I have the same thing here. If you need to edit the post, let me know. As long as you're using the MPMASTER post, it's not too tough to get it to spit out the three trailing zeroes with no decimal.

Yeah... the upgrade is CHEAP. It's mostly software. Like I said, mechanically the machine is already there. I would rather have it and not use it than to not have it and wish I did or have a sudden need to. Better resale IMO... better marketability with a Full 4th = more work potential = more $$$ for the wallet.

Having a Full 4th sells. It doesn't matter so much whether or not a customer understands what you have or thinks that his/her parts need a full 4th. Perception sells in this case. Many of them see HMC with Full 4th and think you have what they need.

Now, as for the mechanical/shop advantages:
1) Do you guys use probing? Having a full 4th will allow for B-axis compensations/corrections. In otherwords, if your part is not square to the machine, probing can correct it. While you can still do this with a 360k positioner, it's not automated by program. It becomes a manual correction. I have written probe cycles to work with the Positioner, but the program format will require a variable in the B moves instead of a direct position. Plus, you'll need to modify the probe cycle to write to a system variable other than a work offset (since you don't have a B offset). The benefits pay for itself in a hurry...

2) Double check this but there's also a safety consideration. I believe the positioner (as well as an indexer) cannot be put into FEED HOLD. So, when the table starts to rotate (for example when you're setting up), FEED HOLD (Cycle Stop) won't stop the table. If you accidently have something or the part in the way, the table will continue and you will crash unless you're quick to hit the E-Stop button.

3) Having a Full 4th will allow you to upgrade software for Dynamic Comp. This will allow for center of rotation programming and the machine/control can adjust for any part positioning errors. Now, the HCN isn't a very large machine so accurately positioning and very repeatable setups are for more easier than a 1000mm + machine, but this can also be used as a preventative measure of miss loads or parts that require loose positioning.

4) Fourth axis contouring has more advanatages than just making a trick looking part. There are processes you can add for better tool blends, ability to make "probe cuts" on the face for rotated work offsetting, different method of attacking profiles without adding a bunch of tools or form tools (allows for better magazine/matrix usage for standardized tooling on small mags), etc, etc.

So, even on parts that "don't need" a full 4th to make, I may still use it to gain better efficiencies for secondary processes (like Detail work), secondary manual operations (like angled holes that might be difficult to consistently locate using index methods in the same part set up) and overall visual appeal of the part.

Originally Posted by psychomill

2) Double check this but there's also a safety consideration. I believe the positioner (as well as an indexer) cannot be put into FEED HOLD. So, when the table starts to rotate (for example when you're setting up), FEED HOLD (Cycle Stop) won't stop the table. If you accidently have something or the part in the way, the table will continue and you will crash unless you're quick to hit the E-Stop button.

YES this it correct. Not only will it NOT feed hold, but the table is always at 100% rapid!