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:

Chip thinning calculator for HSM here...


danielm
 Share

Recommended Posts

Depends alot what you are doing on what machine how much memory you have and so on.

Because most of my machines do not have possibility to work with huge programs and because hsm can not produce subroutines(even while we have this option in operation parameters )I work aggressive with sidecuts I mean they are relatively huge and feeds relativly small

Most folx here use smaller sidesteps and faster feeds .

My message is this all this is very dependant of your local conditions

Test your conditions and find what way to choose smaller cuts and faster feeds or big cuts and relatively small feeds

It works great both ways

My operators love HSM it is fast and great tool life .

I use it on everything from alluminium to stainless .

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

I still have yet to find the hsm/ dynamic toolpaths that have the switch for chip thinning and the different style end mill such as the VRX from Garr. I it Opti-Rough and Opti- Core? Or just Dynamic 2D toolpaths? I just went to a seminar that showed X8 being used but the instructor said the chip-thinning, and slide bar for dynamic milling is in X7. I was impressed with the feeds and speeds but I can't see how to duplicate the results here. Any help is appreciated.

Link to comment
Share on other sites

Switch over to the Iscar Library and you will then see a Iscar HEM check box appear. Click on that and the slider will now function. This ability was only activated with their tools and not others, but you can use it and then redefine them and make up your own library of tools from other manufactures. A little more work, but if I understand correctly per their agreement with Iscar had to be done this way.

Link to comment
Share on other sites

Please post up any questions you have and start off with 100% depth 10% step over with at least .005 to .006 per tooth chip load and max RPM's recommend for your material. Yes you will not be competitive. I helped a customer last week realize a 47% cycle time reduction in their parts. Other customers have seen upwards of 80% reduction in cycles times using the HST toolpaths. Insert manufactures are not all that happy about them, but the solid carbide makers sure are.

 

I have been pushing 200% step downs with up to .01 to .012 per tooth feedrates and been running out of machine abilities before tool abilities to make the cuts.

  • Like 1
Link to comment
Share on other sites

I ran an application using 3/4" solid carbide, 100% depth and 7% step over, axially 1.75, radially almost 2"

This resulted in virtually stress free results and an increase in productivity of about 300% over plunge and feed cutting; I never would have believed such claims until I actually ran it.

This dynamic milling is really something :)

Link to comment
Share on other sites

I have an IPhone video, as crude as it is, but it does show a brief glimpse of how things should be done.

Where do you want the uploads?

45 mins against 18 mins and, the procedure was stress free :)

Before was a 390 Coromill (11mm insert) 1.25" dia. endmill that started bucking as the depth increased (due to radial loading and recutting chips) - still one of my favourite tools!

After was a 3/4" TiAn solid carbide end mill that just ate this application up.

The video was recorded so that our programmer could see this example of dynamic milling in a real application - which was actually ours.

The intention of this video was not for any other reason.

Kudos to Jason Sheldrick of Elliott machine sales in Oakville Ontario for programming it for us.

BTW, the Matsuura MX520 sold 11units in the last 3 months - now that's a quality statement that really delivers!

Link to comment
Share on other sites

Yes the 390 has been a staple for so long, it's hard to convince to go to solid carbide...but man does it work in most applications. Numbers and videos prove it!

 

I've been thinking of adding video links to the dynamic milling database. People would see the data fields, and then video of the cutting. Could be pretty cool.

 

Any ideas where to put videos and how to manage? (other than youtube I suppose)

Link to comment
Share on other sites

I ran an application using 3/4" solid carbide, 100% depth and 7% step over, axially 1.75, radially almost 2"

 

Am I missing something here? You said 7% stepover and then also said almost 2" radially. I thought radial was the stepover amount? lol.

 

To the OP, I use the HSM Advisor program for my needs. I've been pretty successful with it. I've had speeds in 4340 HTSR with a 3/4" 5 flute endmill doing .06 stepover, 4650RPM and .0376/rev, 1.925" deep and it ran very nice. Could have pushed more except I was in a collet at the time and didn't want it pulling out.

 

  • Like 2
Link to comment
Share on other sites

We use the prototyp calculator (downloadable) for a lot of stuff, even competitors cutters, works on volumetric calculations i.e. depth vs radial step and is a great starting point for the HSM toolpaths. As a lot of people suggest start with about 10% radial and 1-1.5 D for depth - machine dependant of course.

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...