Kampfzentrum

Ideal calculations for non-HSM cutting in MasterCAM

Recommended Posts

New to the forum, first time post; admin feel free to move if in wrong area.

 

I'm using MasterCAM for corebox machining (mold dies for castings) and I'm a novice. I'm looking at feeds/speeds/stepdown/stepover and really need help with the calculations. I'm machining in 3 processes (rough/semi-/finish) and using ball/bull endmills from .750-.093 all carbide. 

 

Now, when I calculate feeds/speeds/stepdown/stepover the common Handbook and HSM calculators all account that the DOC/axial cut is consistent. But because I am slowly hacking away at surfaces, these calculations leave me with busted up/broken tools which I am really trying to avoid. I guess what I'm looking for is a easier way to calculate feeds/speeds/stepdown/stepover that are a bit more conservative.

 

I'm primarily machining on 4140 and 6160.

 

Thanks in advance.

Share this post


Link to post
Share on other sites

what I'm looking for is a easier way to calculate feeds/speeds/stepdown/stepover that are a bit more conservative.

 

 

 

Have a look at HSM Advisor, I use it all the time with great results.

4140 cuts like butter, and I have no experience with 6160 steel... unless that's a typo and you meant 6061 Aluminum.

https://hsmadvisor.com/

Share this post


Link to post
Share on other sites

Have a look at HSM Advisor, I use it all the time with great results.

4140 cuts like butter, and I have no experience with 6160 steel... unless that's a typo and you meant 6061 Aluminum.

https://hsmadvisor.com/

 

It's funny you mentioned the HSM Advisor, it was one of the first resources I stumbled upon. The problem with this calculator is that I am not doing high speed machining, that the DOC/axial cut varies throughout. A long tool (3.000) will snap with the calculations given. It is literally why I wrote this post. Honestly, I'm starting to think I'm in a gray area where there is no calculation, I just need to run cautious and find out what works.

Share this post


Link to post
Share on other sites

I hit up the tool makers website or catalog for speed.  What brand of endmills are you using?

  • Like 1

Share this post


Link to post
Share on other sites

You need to get your tool Rep in.  Make him guarantee his parameters, so if you toast it, it'll be on him.

  • Like 1

Share this post


Link to post
Share on other sites

It's funny you mentioned the HSM Advisor, it was one of the first resources I stumbled upon. The problem with this calculator is that I am not doing high speed machining, that the DOC/axial cut varies throughout. A long tool (3.000) will snap with the calculations given. It is literally why I wrote this post. Honestly, I'm starting to think I'm in a gray area where there is no calculation, I just need to run cautious and find out what works.

You can turn off the calculations for HSM and Chip Thinning with that calculator.

 

Learning the speeds and feeds can be a Catch-22. You need experience to know how fast to run the tools, but learning that comes from experience.  :laughing:

  • Like 2

Share this post


Link to post
Share on other sites

I think this might be the problem, we use a substandard tool from a company that regrinds. The tools are always unmarked and reground. They ARE carbide, but I have no data on helical angle etc.

Share this post


Link to post
Share on other sites

I think this might be the problem, we use a substandard tool from a company that regrinds. The tools are always unmarked and reground. They ARE carbide, but I have no data on helical angle etc.

 

Well you are asking for all kind of trouble. Like working with grenade if you ask me. I would never cut 4140 without knowing what the tool and coating was. Doing so is playing Russian Roulette. I had an owner bring me some China endmills one time when I was in a tool and die shop. He paid $6 each for them. After about the 15 endmill wouldn't take a cut he finally listened and we showed him under the Lupe they had a reverse grind on them. The outside was hitter before the cutting edge was.

  • Like 2

Share this post


Link to post
Share on other sites

If you're using a quality tool and HSMAdvisor you should be able to just set the depth and stepover of your heaviest cut.  The numbers are actually pretty good, but you have to use a quality cutter.  If you absolutely have to use your budget cutters you can use 70% or 50% or whatever you need to to keep from breaking the tools and muddle through the job.  Using cheap tools is expensive.

  • Like 2

Share this post


Link to post
Share on other sites

It's funny you mentioned the HSM Advisor, it was one of the first resources I stumbled upon. The problem with this calculator is that I am not doing high speed machining, that the DOC/axial cut varies throughout. A long tool (3.000) will snap with the calculations given. It is literally why I wrote this post. Honestly, I'm starting to think I'm in a gray area where there is no calculation, I just need to run cautious and find out what works.

HSMAdvisor is not only for HSM machining.

Because of a very scientific approach I built into it, it will very accurately tell you what the tool can handle.

 

It especially shines when you need to get proper DOC/WOC for long tools.

 

Obviously for it to work you need to accurately enter as much info about the tool as available. But if tools are "mystery" just use Generic Endmill tool type with whatever coating you think it has.

 

Steer away from "Roughing HP Endmill" if you are not sure.

  • Like 3

Share this post


Link to post
Share on other sites

I'd recommend avoiding mastercam pocket toolpaths and stick with dynamic/HSM toolpaths, if the machine can handle it. Much quicker for hogging out lots of material, it uses more of your cutting edge, the tool keeps more consistent engagement, etc. Just be careful with those back feed moves if you have look ahead... 

  • Like 2

Share this post


Link to post
Share on other sites

If your using a offset geometry toolpath approach(contour, pocket, circle mill, etc) The toolpaths ability to engage a consistant chip load is out the window honestly. A dynamic based toolpath with properly calculated speeds, feeds, and stepover will carry your needs here. You will always bind up a cutting flute in any offset geometry based tp involving a direction change in a corner the size of the cutting tools radius, no matter the quality grade of tooling used. I cut 4140 pre hard easily and trouble free with a dynamic tp at any d.o.c., using a carbide 4flute, AlTin coated gaar vrx, with airblast for chip evac. 350sfm and .002-.004chip/tooth to start and increase ipm from there. I use 20% stepover on low side, adjust the min max arc radius according to cutter size, back feed at 300imp, microlift .01, finishing the floor depth and leaving .005/side stock on walls. I'll come back in with basic contour tp to finish walls, and leave .0003-.0005 on floors to avoid any rubbing/ undercutting on already finished floor. If the floor requires a better finish then dynamic gives, then leave .005 on floor then come back and multipass to depth with a contour tp leaving .005 on walls then finish walls after. It's never a bad idea to float walls with a multipass with a finish pass 1(or more)with a stepover 0.0. I like to jump sfm up to 450-500 on finish ops too.

Share this post


Link to post
Share on other sites

Are you familiar with Opti Rough and Opti Rest?  It will give you dynamic toolpaths with step downs.  ORough with .750, then Orest with smaller end mills.  The rest cleans up what the rough could not reach.  If you know this I apologize.

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