Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

fanuc 16mb high speed machining


Recommended Posts

Hello there,

I am new here , and I have no much experience with HSM , that's why I am asking here, hope I will get some help!

I have been trying hard to get high speed machining right on my Robodrill T10b with fanuc 16mb, I do have G08 function, but machine is still very jerky even @40 ipm, I am running an high speed toolpath.

I am drip feeding program.

Cad cam software is outputting Gcode mostly in g2/g3 output with some small movements between g2/g3 , when machine moves in g2 and g3 and on long g1 movements it's very smooth!

I am not totally sure, but I believe it's not a problem with CAM software...

G64 is active too.

Are there any parameters that can be tuned to improve the motion?

Anybody knows if g5.1 q1 can be an option that can be bought on this Fanuc 16mb? Does it need a software or hardware upgrade , it does not mention this very well on the manual I have.

Thank you guys for the time in advance ,

Regards

Link to comment
Share on other sites

You're trying to drip feed a HS program?

What baud rate?

Chances are most likely your data transfer isn't fast enough...with a Fanuc control you should be able to use the data card option....search this site for Fanuc Data Server....

Link to comment
Share on other sites

These could be the parameters you're looking to "tweak"

1768 (Time constant for Acc/dec AFTER interpolation)
1771 (Time constant for Acc/dec BEFORE interpolation)
 

Depending what they are, you could increase them which will smooth the motion.

You may also have a "Jerk" parameter too. The 31 control has and I had to increase that on my machines when I had them.

 

  • Thanks 1
Link to comment
Share on other sites

Agree with everyone on the above... In my experience drip feeding HSM code usually doesn't work very well, the download can't keep up with the speed of code execution. If you can get away with it might try opening up your arc filters a little more to see if you can get less code to stream, that is, if you can't figure out how to run it off the control or from a memory card that would be best option.

 

If it's a one off piece, you might also consider breaking up the program into sections and running it in smaller chunks that will fit on the control.

Link to comment
Share on other sites

Hi

Thanks again for all the replies, I was not expecting so many!:)

I know that for hsm , drip feeding might not be the best solution, however I am feeding machine at 100ipm max , so I believe is not super fast... to me it seems the control process the code fast enough, but machine struggles on small movements/ changes of direction/ spline execution.

I think that as I also tried tp run a small part of program with those small g1 movements , splines etc, but I couldn't notice a difference.

Once my pcmcia card arrives I will try to drip feed from card.

 

Link to comment
Share on other sites

Newbeeee , I checked those parameters on my manual but I could only find paramters before interpolation , and during cutting feed in look ahead mode...

I will take a picture of the ones you mentioned , as I am not sure what values I should change them to.

What parameter number could be the one for jerky motion?

Can this tuning damage servos?

Thanks for the help

Link to comment
Share on other sites

Here's a detailed link with some other links off of it.

But it's for a 0imC  control. But the parameter description will be the same or similar.

You shouldn't hurt the machine as you're slowing things down. Take notes of where you are before you start and good luck

http://www.practicalmachinist.com/vb/cnc-machining/fanuc-hsm-g08-g05-1-settings-171099/

Link to comment
Share on other sites

Hi ,

I checked the parameters 1768 and 1771 and they are set @ 20 and 80 , can I change them with any number , or is there a criteria to change them? I .e . multiplies of 2 /4 ..... etc...

Sorry for the silly questions , but I actually never done this before.

I couldn't actually find parameter 1769 , it seems like it does not exist , but it seems the most import one too.

 

 

Link to comment
Share on other sites

WOW! it was 9 years ago I played with this...

Here's my Robodrill notes:-

 

Both machines banged using mastercam HS toolpaths when changing direction at high speed (short moves). This was using G05.1.

Ref Fanuc HSM parameter book, the following parameters were changed:-

 

1769 Time constant (ms) for acc/dec after interpolation

Std value was 24, now 50

 

1772 Time constant (ms) for acc/dec before interpolation

Std value was 48, now 150

 

Both these machines had 31 controls so the parameters are different. But you can see how they were opened up which doesn't affect accuracy.

 

But, as you have the older 16 control and the 0imC was based on that architecture, I'd go for:-

1768 Was 20 / Now 50 (you have lighter table and Alpha drives/servos so faster response than the bigger Chevalier machines that the links were based on)

1771 Was 80 / Now 150

 

Give it a go and see but I think your main problem is drip feeding so you should be running off your M198 memory card 

Link to comment
Share on other sites

Hi ,

I haven't had the chance to tweak parameters yet.

I could be wrong , but I think I found the equivalent of param 1769 on 16 MB.... looks like param 1762 ( I could be wrong).

So would be 1762 , 1768 ,1771.

Param 1762 , is all set to 0 at the moment.

Attached the screen shoots with param description.

My 2mb pcmcia card should be coming today :) I got it in order to back up my parameters , but I am not sure if control can drip feed from memory card.

I spent few hours yesterday on the books , and it seems that G05.1q1/q0 does not exist in this Fanuc ... only g08 , g05 p10000 :(

 

 

PARAM 2.jpg

PARAM 1.jpg

PARAM 3.jpg

Link to comment
Share on other sites
  • 4 weeks later...

Hello there ,

 

I tried only today to switch those parameters and machine is moving much smoother!! :):):):)

I am so happy! you can still see the machine slowing down , but motion is smoother , and you don't hear any banging :):)

Any other paramter I can change or any other suggestions?

I am upgrading my machine memory next to week , with a 2mb module.

Regards 

 

Link to comment
Share on other sites

I will as soon I have the chance!

I am only interested on "hsm" only for roughing purposes , I still don't understand why the difference in motion between a simple normal tool path and this trochoidal style machining ,, could it be the small movements?It slows down up to 30% of the programmed feed rate , but now without banging so is already better than before.

Any other tweaks suggestions I could do? 

I am not sure if parameter 1762 I posted previously could be any good to be changed?

Anyway , I am happier than before , thanks again!!!!!!!

I will keep the forum updated!

  • Like 1
Link to comment
Share on other sites

Hello Sticky,

 

As said before, I am installing the 2mb memory upgrade this weekend,so I will be running programs from memory. Have you got a suggestion for changing other parameters?

From other emastercam posts there seem to be another parameter called allowable velocity difference in velocity determination considering the velocity difference at corners.

As said before , now machine is not banging anymore , which is a good result , but on those small movements machine still slows down a lot up to 10% of the programmed feed rate.

I think tool path I am running as micron tolerance , certain movements differ between them for just .008mm.

Again, any suggestion?

Many thanks to all in advance! 

Link to comment
Share on other sites
9 hours ago, Poxino said:

As said before , now machine is not banging anymore , which is a good result , but on those small movements machine still slows down a lot up to 10% of the programmed feed rate.

 

If it only slows 10% but is not shaking itself to bits, and is still accurate, call it a result and make parts!

Link to comment
Share on other sites

Hi,

Maybe I did not word the sentence properly, I meant is slowing down up 10% of the programmed feed rate , just to give you am example programmed feed rate 2500(100ipm)mm/min and actual feed rate 250 (10ipm)mm/min.

This was happening also before changing the parameters above.

But, as said machine is not banging anymore, which is already something.

I am not sure if there are other parameters I could have a look at?

Thanks again

Link to comment
Share on other sites
10 hours ago, Poxino said:

Hi,

Maybe I did not word the sentence properly, I meant is slowing down up 10% of the programmed feed rate , just to give you am example programmed feed rate 2500(100ipm)mm/min and actual feed rate 250 (10ipm)mm/min.

This was happening also before changing the parameters above.

But, as said machine is not banging anymore, which is already something.

I am not sure if there are other parameters I could have a look at?

Thanks again

Ohhh, that is excessive...

There are other parameters - i'll have a look and get back to you.

Link to comment
Share on other sites
On ‎6‎/‎15‎/‎2018 at 12:38 PM, Poxino said:

I am only interested on "hsm" only for roughing purposes , I still don't understand why the difference in motion between a simple normal tool path and this trochoidal style machining

It's not the feedrate in the code that is slowing you down, it is the sheer volume of code being processed through the DNC (Dripfeed).

What are your Line/Arc filter settings?

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...