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:

Problem with Dynamic Core Milling


AMF
 Share

Recommended Posts

The cutting portion of the toolpath is controlled by the "Stepover" parameter.  The toolpath that you have there looks good.  It is common to see the radius moves appear larger than the linear.  The toolpath maintains a consistent tool engangment not necessarily an exact step over amount. 

Link to comment
Share on other sites

AMF,

 

The Dynamic Toolpaths are designed to maintain a constant engagement with the material. Going around a sharp corner like that, the tool needs to expand outwards to be sure that you aren't over-engaging the material. John is right, that toolpath looks ideal.

 

Are you actually having problems running that path on the machine? What kind of geometry did you use? Can you post up a copy of the toolpath with only the wireframe chains you used to drive it?

Link to comment
Share on other sites

We haven't ran the part.  The part is steel, and we are anticipating trouble with this toolpath.  We are wanting to run full axial ( 1.00 DOC ), with a .875" carbide endmill.  I have generated just a core toolpath, and if it didn't retract constantly it is just what we want.  I have attached the file.   What do you think is the best option for this part? 

 

Thank you very much for your help!  

 

AMF

CORE.MCX-7

Link to comment
Share on other sites

If you look at the "Important Topics" at the top of the forum that JP made, there is a link to the Dynamic Milling database that Chris Rizzo maintains.

 

For 1018 CR steel, it looks like people are running about 800 SFM.

 

I set up this Dynamic Core path to use about a 10% stepover, and to not retract the tool. (The tool stays down using a micro-lift move at a higher feedrate.)

 

This will work great for a full flute-length cut, especially since you are at about 1:1 depth to diameter ratio.

 

Just keep in mind that this path isn't a finishing toolpath. I left .01 of stock, so that you can clean it up with a contour toolpath.

 

You should be around 3500 RPM, and 120 IPM.

 

Hope that helps,

 

Colin

CG_CORE.MCX-7

Link to comment
Share on other sites

Wow, that seems really fast to me, but I'm going to give it a try.

 

Thanks Colin and JParis.

 

 

 

AMF

 

Yes, it should seem fast. That is what you gain from using the Dynamic motion.

 

Keep in mind though, you need to have a nice rigid tool holder, that spins true, and the part should be very secure on the table.

 

If you are holding your tool way out from the holder, and using a side-lock holder with set screws (pushing the tool out-of-round a little bit), then you might need to reduce those values somewhat.

 

Check out that Dynamic Milling Database. It is in spread-sheet format, and has entries from many different people for starting values. There are probably 8 different entries for 1018 CRS.

Link to comment
Share on other sites

Perfect timing. Last night we were testing the limit of  what a 1/2 cutter, .875 deep would do in 1018. Tool broke at 750 ipm at 6000rpm.  10% stepover.  Imco pow-er-mill tool.

 

HIGHLY recommended use x8, because it has first pass offset and feed reduction. Those are two must-use features for rectangular shape stock. Otherwise over engagement in corners = tool breakage. I'm assuming that's what you were referring to in your picture? The increased corner engagement?

 

A few of my latest findings: Only use micro-lift if the floor matters. Even the fastest machine will decel coming in and out of a micro-lift. Keep filter tolerance at .001 regardless of stock to leave. Any value larger and tangency between moves goes away, thus machine decells a to minimize overrun. I'm working with an Okuma Geno OSP 300 with super-nurbs, so I've got the control and machine to digest these rates.

 

My goal is to cut at 1000ipm.

Link to comment
Share on other sites

I just had this same issue on a mold core. I sent it in to In-House who then passed it along to CNC Software. Although they did get back to me, I'm not satisfied with the reply. In a nutshell, they basically said what was written above, that the tollbooth tries to maintain constant tool load. I call BS on this. The toolpath is supposed to be controlled by "stopover" as its criteria. We had areas of our part where the stopover was just a tad over double what we programmed for stopover. Yes....... this is BAD for the tool. Seeing as "stopover" is the only control you have for this path, my thinking is that it should have a "minimum" and "maximum" stopover value. It's an awesome toolpath, but certainly has some short-comings in my eyes.

 

Carmen

Link to comment
Share on other sites

Imo as the cutter rolls around the corner, its effective feedrate will be smaller than the programmed one and thus some over-engagement is acceptable.

ALSO when you cut outside arc, the effective width of cut will be smaller than the programmed offset! and the effective with of cut will be smaller than what you see on the screen.

 

Also CAM can not have CONSTANT engagement all over the part anyway. You still need to take light leadins, leadouts etc.

 

Also what you see on the screen sometimes is misleading.

Example: if cutter attacks pocket from both sides it may appear on the screen that in the center the cuts are extremely heavy. but in fact it is not true as there is no more material left from the previuous passes.

 

Link to comment
Share on other sites

If you backplot and save as geo, you can analyze and see the user-entered stepover value is violated. Period. Not by a bit, but sometimes 40-50%.

 

 After a few passes and the sharps are knocked off and the morphing gets going, and stepeover is NOT violated, and the toolpath becomes "correct".

 

Inside corners it stays at the programmed stepover, and rounding radius.

Link to comment
Share on other sites
If you backplot and save as geo, you can analyze and see the user-entered stepover value is violated. Period. Not by a bit, but sometimes 40-50%.

 

 After a few passes and the sharps are knocked off and the morphing gets going, and stepeover is NOT violated, and the toolpath becomes "correct".

 

Inside corners it stays at the programmed stepover, and rounding radius.

I just added to the post above that when cutter does an arc on the outside, its effective WOC WILL be smaller than the distance between the passes.

 

Google "circular interpolation effective with of cut"

Link to comment
Share on other sites

The first pass offset and feed reduction are clever patches, but just that, patches. They don't address the over engagement. I'm curious what volumill and other software packages look like in this situation.

 

I spoke with one of the guys that works at Volumill during IMTS. Ironically, they are also located in Connecticut, along with CNC Software. He mentioned that their software varies the feedrates for each block, along with controlling the stepover. So in some instances, the tool will just slow down. They also create some different types of tool motion in tight areas. Where Dynamic Mill will just reduce the stepover into small slots, Volumill will pick the tool up, and make slotting passes in-between the tight areas, at a reduced depth of cut.

 

I don't have any personal experience with using Volumill, but the features the guy was describing sounded like they could be very useful.

Link to comment
Share on other sites

I spoke with one of the guys that works at Volumill during IMTS. Ironically, they are also located in Connecticut, along with CNC Software. He mentioned that their software varies the feedrates for each block, along with controlling the stepover. So in some instances, the tool will just slow down. They also create some different types of tool motion in tight areas. Where Dynamic Mill will just reduce the stepover into small slots, Volumill will pick the tool up, and make slotting passes in-between the tight areas, at a reduced depth of cut.

 

I don't have any personal experience with using Volumill, but the features the guy was describing sounded like they could be very useful.

 

 

I cant tell you how disappointed I was when Mastercam dropped Volumill.  Dynamic milling is awesome, but Volumill exceeded in areas that Dynamic failed. Neither were good for every single situation.

 

I still have a bunch of Volumill paths in old part files. Ive had to save the NCI and import it in to new versions of Mastercam which sucks.

Link to comment
Share on other sites

RE: Dynamic Milling Database...

 

Chris, is there a way to make the left side row headings stick and have the rest of the data scroll horizontally? As soon as you scroll, the headings disappear and that makes it a pain to figure out what data is what.

 

THANKS for putting something like this together! It's a great resource! :unworthy:

  • Like 2
Link to comment
Share on other sites

RE: Dynamic Milling Database...

 

Chris, is there a way to make the left side row headings stick and have the rest of the data scroll horizontally? As soon as you scroll, the headings disappear and that makes it a pain to figure out what data is what.

 

THANKS for putting something like this together! It's a great resource! :unworthy:

 

 

yeah, that would be great. 

Link to comment
Share on other sites

RE: Dynamic Milling Database...

 

Chris, is there a way to make the left side row headings stick and have the rest of the data scroll horizontally? As soon as you scroll, the headings disappear and that makes it a pain to figure out what data is what.

 

THANKS for putting something like this together! It's a great resource! :unworthy:

 

Thad, check out Chris' signature: ..(Google Chrome will freeze the first column, IE and firefox won't)

 

Just use Google Chrome to view the spreadsheet, and the first column freezes...

Link to comment
Share on other sites

I just had this same issue on a mold core. I sent it in to In-House who then passed it along to CNC Software. Although they did get back to me, I'm not satisfied with the reply. In a nutshell, they basically said what was written above, that the tollbooth tries to maintain constant tool load. I call BS on this. The toolpath is supposed to be controlled by "stopover" as its criteria. We had areas of our part where the stopover was just a tad over double what we programmed for stopover. Yes....... this is BAD for the tool. Seeing as "stopover" is the only control you have for this path, my thinking is that it should have a "minimum" and "maximum" stopover value. It's an awesome toolpath, but certainly has some short-comings in my eyes.

 

Carmen

 

 

The first pass offset and feed reduction are clever patches, but just that, patches. They don't address the over engagement. I'm curious what volumill and other software packages look like in this situation.

 

 

Hey guys,

 

Since you are having a problem with the over engagement in the corners, check out what happens if we use the ModuleWorks "Triangular Mesh" toolpath to do Dynamic milling. (In the MW interface, sometimes they use Adaptive in place of Dynamic.)

 

In the MW interface, they actually do give you a "desired" stepover value, and a "Max" value. (the numbers seem to be tied together, change one, the other updates, so you can't use them independently)

 

One of my favorite things though is the ability to do Zig Zag cutting, and specify a different percentage of the desired stepover for climb vs. conventional. I'm not sure this would work in Ti or any of the harder materials, but it works awesome when cutting aluminum, as you aren't wasting time backfeeding, you are always cutting material.

 

One final option I used for both example paths is the "Feed Control Zone". I created some square solids near the corners of the part. As the tool passes through these solids, the path slows the feedrate by 50%. Once clear of the FCZ solids, the path speeds back up to the normal cutting feedrate.

CORE_MW_ADAPTIVE.mcx-8

CORE_MW_ADAPTIVE.MCX-7

  • Like 2
Link to comment
Share on other sites

Been busy all day- missing out on the fun here...

 

Yes the first column not locking really makes it a hassle to view the information. Chrome browser will lock the first column, and firefox might now. (It behaves a bit different for me because of full edit permission). Now that I think of it, I need to go in and organize some recent entries. (The google auto-entry form will only output a horizontal format spreadsheet,  which is nearly unreadable. I have a shell that re-formats it into the legible vertical format and fancy colors).

 

Been wanting to try that triangular mesh for a while, you've been really talking highly of it, thanks for the example file Colin.  Interesting if you change the "Type" from adaptive to parallel, you get a completely different toolpath. Lots of options in there. I really need to set aside some time this Xmas break and learn it.

 

Oh, this is back in X5 when I learned about the over engagement "issue"....with a $200 Sandvik Plura Mill.

 

 

 

IMAG0049_2.jpg

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...