Ewood42

haas tool length system macro variable #s

Recommended Posts

Sorry if duplicate post, but does anyone know what # range these use? I'm trying to get more tool life out of a 1/4" x 1/2" flute endmill we're profiling sheet metal with. Really only using about .1" of the flute, seem like a shame to not use more. Going to set up a counter to increment the length .05" deeper each cycle until it hits the last of the flutes on the 7th cycle and reset. Need to be able to write directly to offset register with a macro to do so.

 

Edit - legacy #2001-#2200 for length, #2201-#2400 for wear (L)

  • Like 1

Share this post


Link to post
Share on other sites

Could you just do the same thing with the Z in the program? 

Share this post


Link to post
Share on other sites

Why not use 2d oscillate dropdown in contour which is specifically for this application?

Share this post


Link to post
Share on other sites
16 hours ago, Codeworx said:

Why not use 2d oscillate dropdown in contour which is specifically for this application?

I already am, but the short length of some of the contours and the ramp angle imitations of the tool (not to mention the excess chatter when you use a high osicllation angle) it is of limited use and can't be set higher than .06" across .60" without adversely affecting tool life.

I just tested out an endmill that outperforms what we had been using, but it does not come in stub length as a standard. a custom stub is about the same price- so why not try to get full use of that 3/4" flute length?

 

17 hours ago, navsENG said:

Could you just do the same thing with the Z in the program? 

I thought about outputting 4 versions of the file and just cycling through them as sub program calls, but then if I want to tweak any of the parameters I have to go back to my desk and repost. Now, if we want to test another tool or different step increment/frequency, I just change a couple parameters at top of file and it's done.

I got it sorted out. Having it adjust the wear length offset instead of tool length to avoid having to track the original # and avoid any potential problems if it gets reset midway through. Also added some idiot proofing so if I fat finger a parameter it will alarm before running.

 

I have another part we make tons of that I do something similar with. We were getting 25 parts to an endmill, but the minimum flute the tool had was about 10x material thickness. So now we step down half the material thickness every 10 parts and use the whole flute length, getting about 200 parts per tool instead now.

  • Like 3

Share this post


Link to post
Share on other sites

G10

Share this post


Link to post
Share on other sites
5 hours ago, Ewood42 said:

I already am, but the short length of some of the contours and the ramp angle imitations of the tool (not to mention the excess chatter when you use a high osicllation angle) it is of limited use and can't be set higher than .06" across .60" without adversely affecting tool life.

I just tested out an endmill that outperforms what we had been using, but it does not come in stub length as a standard. a custom stub is about the same price- so why not try to get full use of that 3/4" flute length?

 

I thought about outputting 4 versions of the file and just cycling through them as sub program calls, but then if I want to tweak any of the parameters I have to go back to my desk and repost. Now, if we want to test another tool or different step increment/frequency, I just change a couple parameters at top of file and it's done.

I got it sorted out. Having it adjust the wear length offset instead of tool length to avoid having to track the original # and avoid any potential problems if it gets reset midway through. Also added some idiot proofing so if I fat finger a parameter it will alarm before running.

 

I have another part we make tons of that I do something similar with. We were getting 25 parts to an endmill, but the minimum flute the tool had was about 10x material thickness. So now we step down half the material thickness every 10 parts and use the whole flute length, getting about 200 parts per tool instead now.

I meant just use a variable for your Z depth and increment that variable with a counter. I do that all the time with extra face stock. Use the probe to calculate how much extra stock the part has, and it will calculate the starting Z and all the incremental passes. 

I just don't like to mess with the tool length because if you ever wanted to use the tool for something else, it could be dangerous..

But as we know in this industry, many ways to achieve the same outcome....

Share this post


Link to post
Share on other sites

FYI, Its in the Operators manual if your looking for a full list.

image.png.d38f2bae40072b73628f29a1d1c88962.png

Share this post


Link to post
Share on other sites
On 7/20/2019 at 10:41 AM, Codeworx said:

FYI, Its in the Operators manual if your looking for a full list.

That's exactly what I eventually found and printed out.

 

On 7/19/2019 at 3:34 PM, navsENG said:

I meant just use a variable for your Z depth and increment that variable with a counter. I do that all the time with extra face stock. Use the probe to calculate how much extra stock the part has, and it will calculate the starting Z and all the incremental passes. 

I just don't like to mess with the tool length because if you ever wanted to use the tool for something else, it could be dangerous..

But as we know in this industry, many ways to achieve the same outcome....

That would be a lot of Zs to change... I had a hard time finding and adjusting all the R planes to use a variable. Did I mention it was an oscillating contour in a 5 axis mill program and only 2 of the 6 cuts are actually a straight line?

No worries about causing problems with other parts though. This one part is literally all that machine ever runs, and all it ever will for at least another 4 years. That's why I get to spend so much time on process improvement for that one part- there's still plenty of time for it to pay off.

  • Haha 1

Share this post


Link to post
Share on other sites
4 hours ago, Ewood42 said:

That's exactly what I eventually found and printed out.

 

That would be a lot of Zs to change... I had a hard time finding and adjusting all the R planes to use a variable. Did I mention it was an oscillating contour in a 5 axis mill program and only 2 of the 6 cuts are actually a straight line?

No worries about causing problems with other parts though. This one part is literally all that machine ever runs, and all it ever will for at least another 4 years. That's why I get to spend so much time on process improvement for that one part- there's still plenty of time for it to pay off.

Ahh yes, only a few thousand Z offsets to change no big deal..... haha 

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now

  • 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