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:

hurco post help again


petro7
 Share

Recommended Posts

Sounds like the post is working fine.

Do This:

Retract .1 -  This can be absolute for flat plate. Incremental for different heights  of picked geo.

Clearance 2.0  absolute to jump over clamps. Inc if you jumping to different heights of geo.

 

Look at the screen and watch what it does. The line color -Yellow for rapid, blue for feed.

Play with it and watch the path. Make sure you turn the icons on for rapid so you see the moves.

Link to comment
Share on other sites

CHeck this out

 

These settings, will get you

 

Jump_01_zps86eb538b.png

 

This

 

Result_01_zps28d95ed8.png

 

NJow right click go to Toolpath editor

 

Jump_02_zps817f5eea.png

 

Select the point to jump at

 

Change_01_zpsd12abd76.png

 

Set your Jump height for that point, note the settings for only or all following

 

Jump3_zpsc78fc493.png

 

Toolpath goes dirty, regen and get this

 

Jump_04_zps6dc6cc24.png

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

still having trouble with drill and tap cycles, can some look at this code and see if it looks right. z rapid  to 2.0 , then to .1 ,then to z0. then it start to feed. we tried to set it the same as J paris said but it will still rapid right to z0.

 

(T)
(MASTERCAM - X)
(MCX FILE  - T)
(POST      - )
(MATERIAL  - ALUMINUM INCH - 2024)
(PROGRAM   - T.NC)
(DATE      - FEB-20-2015)
(TIME      - 11:03 AM)
(POST DEV  - IN-HOUSE SOLUTIONS)
(T1  - 13/64 DRILL          - H0  - D0  - D0.2031")
N100 G70 G75 G90
N110 G00 T1 M06 (13/64 DRILL)
N120 (MAX - Z2.)
N130 (MIN - Z-.3)
N140 G00 X0. Y0.
N150 S2800 M03
N160 Z2. M08
N170 Z.1
N180 G81 Z.4 R.1 F8.
N190 X.5 Z.4
N200 X1. Z.4
N210 G80
N220 Z2.
N230 M09
N240 M05
N250 G00 M25
N260 M2
E

Link to comment
Share on other sites

We had a very old Hurco post that did the same thing.  It would start drilling at your retract height which is fine until you want to move over clamps; setting the retract height to 1 inch meant that it would start drilling 1 inch above the part.  If we used the Clearance plane, it would add the clearance plane to the drill depth.  So if I put in a clearance plane of 3 inches it would want to drill 3 inches deeper.

 

I would contact your reseller and have them look at it or have them send you a new post.

Link to comment
Share on other sites

Dave do you run Hurco? for some reason with Hurco when drilling  Z+ is into the part.  also everything is incremental from where you start. so if you start .1 up in z you have to tell it drill .5 deep to get a hole .4 deep. maybe there is a machine parameter to change that i don't know about. but we have been running this way for a few years now. maybe some of the Hurco guys here have a different way to do this. dave this is the confusing part. you have to position Z to the staring height. so you would start Z @. 2   then your R would be .1 , then the machine would start drilling at .1 then retract to .2 to move to the next hole. I am open for suggestions if this is not right.  Cheers

Link to comment
Share on other sites

ITs not just the Post. That  Hurco has 3 levels of NC programming software.

The first one is standard

The next two are add ins. $$ you spend for a disk that adds it  the main software. The Hurco dealer handles this. It has to be mailed to you.

No downloads allowed. Its tied to the serial #, which you have to give them.

 

Now, my point is those 3 levels are all different in how the Hurco handle nc code.

Level 3 will work just like a Fanuc.

 

The other 2 ( built in and level 2) leave a lot out, so you have to be careful.

I haven't run one in while, but drill functions are weird.

 

Do you have any idea what level you have?   Call the dealer for some help. He can explain how it works for the NC level you have.

 

 

Machineguy

.

Link to comment
Share on other sites

Bnc is what comes in the machine

ISNC is the full on package. It will setup just like a fanuc as far as TLO, and work offsets. You can even do bottom up programming on it.

What I mean by that is I usually start working from top to bottom first. 

If I need to flip the part over Z0 is now on the bottom. BNC wont let you do that. There is also a few other quirks.

 

I learned to do things on a Hurco that  the dealer didn't know you could do. It took a while to get good at it as there was a lot to remember  in a conversational pgm.

Link to comment
Share on other sites

Dave do you run Hurco? for some reason with Hurco when drilling  Z+ is into the part.  also everything is incremental from where you start. so if you start .1 up in z you have to tell it drill .5 deep to get a hole .4 deep. maybe there is a machine parameter to change that i don't know about. but we have been running this way for a few years now. maybe some of the Hurco guys here have a different way to do this. dave this is the confusing part. you have to position Z to the staring height. so you would start Z @. 2   then your R would be .1 , then the machine would start drilling at .1 then retract to .2 to move to the next hole. I am open for suggestions if this is not right.  Cheers

 

Petro, No I don't run a Hurco. From the description it sounds like the Z.1 on line N170 may be keeping you from returning to the clearance plane at 2".

But like I said I don't do Hurco just an observation.

Link to comment
Share on other sites

Yes Dave that was 1 of the problems, the other 1 is the r value needed to be 1.9 so then it would rapid .1 above the part drill the hole then rapid back up to the 2 " . drilling with Hurco is a little odd. but once we get the post the way we want then the problem is solved, cheers.

Link to comment
Share on other sites
  • 2 weeks later...
  • 1 year later...

Can anyone give me a sample of program for Hurco VM10 with ISNC package?

I'm interested in tool changes, rigid tap cycle and info on any quirks? Supposedly it'll run a regular Fanuc code.

We just bought it for tool room in a different facility and I'm hoping to set up a post for it so we don't have to use conversational side if we don't want to.

 

TIA

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...