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:

Stepover used in dynamic milling


Recommended Posts

What stepover do you generally use to cut tool steel /mold steel when using dynamic toolpaths? I have seen people using above 25-30% stepovers on youtube. I havent tried these values yet, just wanted to know what is industry standards?  PS i am new to this forum

Link to comment
Share on other sites
1 hour ago, AHarrison1 said:

This will be very much dependent on tool manufacturers recommendations.

 

And other criteria, like workholding rigidity, taper size of the spindle, h/p or spindle, machine-size/rigidity (we can't do 25% on our little Brothers but we can on the DMGs).

Link to comment
Share on other sites
Guest flatcalmproduction

(My first post as well, I am hopeful it will help)

As long as you are using a “Chip Thinning Calculator” the radial engagement (RDOC – Radial Depth of Cut / angle of engagement) can really vary up to 45%. And as AHArrison1 & Jobnt are pointing out, the conditions in which you are cutting will play a major part to your decision.

If your set up is rigid you may see good results at a 25% RDOC or more.

If your out of holder is greater than 4x Diameter, or your set up is not rigid, you may need to run a 10% RDOC or less.

An additional contributor will be the ADOC (Axial Depth of Cut). The flute stabilizes your cut with a shallow RDOC and deep ADOC. If it is a shallow ADOC you may as well increase your RDOC to maintain a high MRR (Material Removal Rate). Shallow depth of cut = deeper radial engagement.

A common oversight you may also consider is “Peak Feed Rate” (how fast the machine is actually moving). You will notice when using the “Chip Thinning Calculator” you are able to increase your feed rate when you reduce your RDOC. The oversight is when a tool path is programmed at 1200 IPM (Inches per Minute) and the machine travel never exceeds 2 inches. The machine may never achieve 1200 IPM. In that case the “Peak Feed Rate” may be used to “reverse engineer” to get the ideal RDOC to use.

Note that one of the benefits/advantages to the dynamic tool paths in Mastercam is that it controls the entry and exit motion. The dynamic tool paths are great to use, even if it is 100% RDOC.

 

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

My general rule of thumb which always depends on the workholding rigitity, tool holder, and the tool geometry itself. I like to use a 5% step over for exotic materials(Inconel and waspoloy) 10% step over for titanium, 15% for stainless,  20% for most steels and 25% for aluminum. This is just starting parameters and there is more to take in to consideration. 

Link to comment
Share on other sites
  • 3 weeks later...
On 6/5/2023 at 12:34 AM, Harshad said:

What stepover do you generally use to cut tool steel /mold steel when using dynamic toolpaths? I have seen people using above 25-30% stepovers on youtube. I havent tried these values yet, just wanted to know what is industry standards?  PS i am new to this forum

This all depends on the ratio of flute length to diameter, and hardness of material, softer materials can be machined with higher stepovers.

With a tool of 2.5xD or less, I run around 10 to 12%.

Over 2.5xD and I run more toward 7 or 8%.

 

Two examples of this would be 6061 Aluminum and 1018 Steel.

In aluminum I usually use a 1/2" 3FL 1.25LOC endmill at 15% stepover, 7500RPM, and 135IPM.

In steel I usually use a 1/2" 7FL 1.25LOC endmill at 10% stepover, 5300RPM, and 120IPM.

Also, remember, tool holder runout is your enemy in HEM, not only will it sound like hell, it will prematurely destroy your tool.

 

  • Thanks 1
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...