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:

2020 Curve 5 Axis


khass0410
 Share

Recommended Posts

Hoping someone can tell me what I'm doing wrong or why I'm not getting the results that I am wanting to get when using the Curve 5 axis toolpath. I've tried using the Curve 5 axis toolpath in the past but I always get steps in between each step over on my parts when using multi-pass. I'm using the bottom of the endmill with plenty of overlap while rotating C axis. The machine this is running on is a 5 Axis Makino D500. 

I've attached a couple pictures. The first picture is when I tried using a 1/2" .060R Mill with a step over of .250" 5 times. The second one is when I tried using a 1.0" .060R Mill with a step over of .500" 2 times. I've also attached my file just in case someone wants to see what have in the parameters. I'd really like to figure out what I'm doing wrong because I normally resort back to using a 3d surfacing toolpath to get the results that I need. Thanks for the help.

.250 EM.jpg

1.0 EM.jpg

Link to comment
Share on other sites

The problem is not your toolpath. The problem is your tool. Your tool is not a perfectly ground flat bottom end mill from what I am seeing in the pictures. You must have the tool specifically made with a perfect flat bottom grind when ordered. Almost every endmill has a slight taper inward to allow center cutting. However in your case when doing 5 Axis it creates a problem like your seeing. The only solution using your tool is to take more steps for the finish pass, but leave the roughing like you have it. Take OP2 and leave .01 on the floor. Take OP1 and do a smaller step over and more passes on your multi-pass if your going to use the tool you got. Be careful with how much weight and places your taking stock off that face mill. I would leave a bigger fillet radius in those corners IMHO.

Please take the time to define your holders.

  • Like 1
Link to comment
Share on other sites

Thought I would offer an alternative way to approach your machining process to see what you thought. Dynamic milling that shape verse traditional milling. Hopefully it gives you some ideas on different ways to machine shapes like this. Have a good day.

Here is a Link to the file. Here is a Video link showing the toolpath in motion.

 

Edited by crazy^millman
Pictures removed to add space
  • Like 1
Link to comment
Share on other sites
1 hour ago, 5th Axis CGI said:

The problem is not your toolpath. The problem is your tool. Your tool is not a perfectly ground flat bottom end mill from what I am seeing in the pictures. You must have the tool specifically made with a perfect flat bottom grind when ordered. Almost every endmill has a slight taper inward to allow center cutting. However in your case when doing 5 Axis it creates a problem like your seeing. The only solution using your tool is to take more steps for the finish pass, but leave the roughing like you have it. Take OP2 and leave .01 on the floor. Take OP1 and do a smaller step over and more passes on your multi-pass if your going to use the tool you got. Be careful with how much weight and places your taking stock off that face mill. I would leave a bigger fillet radius in those corners IMHO.

Please take the time to define your holders.

Ron, thanks for the replies. I came really close to bringing up that the tool I'm using is a center cutting endmill. I was wondering if that could of been the problem, I appreciate the explanation on what is going on. This is a cutter that we are making for a customer, when putting weight reduction on a cutter this is not typically what we do but this is what they want. I agree on the with the bigger fillets. I forgot to put one of Schunk holders on the tool when sharing the file, I sometimes use the holder avoidance tool inside the parameters, so normally I have my holders set up.

The other part that I was working on when having the same problems, I ended up using the multiaxis roughing op to finish. I never even thought about using axis substitution with dynamic milling that's brilliant. Thank you for the help and great ideas.

Link to comment
Share on other sites
33 minutes ago, David Colin said:

There are some valuable info on Sandvik website about turn milling https://www.sandvik.coromant.com/en-gb/knowledge/milling/pages/turn-milling.aspx

They also have available carbide cutters with ground flat (R216.T4)

Thanks for sharing the information, this will be a great resource. I'll have to look up their cutters price range but I can imagine it's going to be more than what our shop will want to pay. lol. But, thanks for showing me what I should be looking for.

Link to comment
Share on other sites
17 hours ago, 5th Axis CGI said:

Thought I would offer an alternative way to approach your machining process to see what you thought. Dynamic milling that shape verse traditional milling. Hopefully it gives you some ideas on different ways to machine shapes like this. Have a good day.

Here is a Link to the file. Here is a Video link showing the toolpath in motion.

 

So the machine we are running these cutters on is a Makino D500 with A and C axis and we use G43.4 mixed with G68.2...... Will axis substitution work with G43.4? or is it meant to come from exact center of pivot? I'm not exactly sure how you set up axis substitution either, I think I have to use the Xform "Roll/Unroll" function to unroll my geometry but when I do it in my main view "how the part is sitting in machine" than I get odd twisted up geometry. I can mimic what you did in the front view but am sort of lost on doing it in my base view....... I will continue working on it any hints would be great though. 

Also work is going to order a couple of them Sandvik Endmills that David Colin mentioned, pretty excited about this. Thanks for all the help you guys.

Link to comment
Share on other sites
4 hours ago, khass0410 said:

So the machine we are running these cutters on is a Makino D500 with A and C axis and we use G43.4 mixed with G68.2...... Will axis substitution work with G43.4? or is it meant to come from exact center of pivot? I'm not exactly sure how you set up axis substitution either, I think I have to use the Xform "Roll/Unroll" function to unroll my geometry but when I do it in my main view "how the part is sitting in machine" than I get odd twisted up geometry. I can mimic what you did in the front view but am sort of lost on doing it in my base view....... I will continue working on it any hints would be great though. 

Also work is going to order a couple of them Sandvik Endmills that David Colin mentioned, pretty excited about this. Thanks for all the help you guys.

G43.4 is for Multiaxis continuous work and G68.2 is for Locked Plane work. As long as you remember the difference then your good. I just gave you an example with FRONT/FRONT/FRONT, but it should work if you use the same base WCS then use FRONT/FRONT. Sometimes the problem is what you see in Mastercam doesn't carry over to the machine so you need to cheat the geometry to get the angles to line up. Where a true CAV is best, but you can run it above the part and then adjust the angle with the machine offset or the position of the chain. Remember this is circumference when unrolled. Take the circumference at the diameter unrolled from and use it to map the angle where this cut is going to fall on your part. Normally it is a 90 degree difference, but I have had to chase 1.7895 degree differences before. The old school way I use to program roll dies is what your seeing happening here. The length of the circumference is your full rotation. Your distance out to at least 6 places if your best control. Now we do the math and come up with a line from zero in the direction we unrolled our geometry that is 53.6791810" long. When we divide this into 360 segments or put 360 points on it each segment represents 1 deg index along the axis of ration we are working with. Now you can move the unrolled geometry exactly where you need it and your in the exact place you need and done. 

  • Huh? 1
Link to comment
Share on other sites
23 minutes ago, 5th Axis CGI said:

G43.4 is for Multiaxis continuous work and G68.2 is for Locked Plane work. As long as you remember the difference then your good. I just gave you an example with FRONT/FRONT/FRONT, but it should work if you use the same base WCS then use FRONT/FRONT. Sometimes the problem is what you see in Mastercam doesn't carry over to the machine so you need to cheat the geometry to get the angles to line up. Where a true CAV is best, but you can run it above the part and then adjust the angle with the machine offset or the position of the chain. Remember this is circumference when unrolled. Take the circumference at the diameter unrolled from and use it to map the angle where this cut is going to fall on your part. Normally it is a 90 degree difference, but I have had to chase 1.7895 degree differences before. The old school way I use to program roll dies is what your seeing happening here. The length of the circumference is your full rotation. Your distance out to at least 6 places if your best control. Now we do the math and come up with a line from zero in the direction we unrolled our geometry that is 53.6791810" long. When we divide this into 360 segments or put 360 points on it each segment represents 1 deg index along the axis of ration we are working with. Now you can move the unrolled geometry exactly where you need it and your in the exact place you need and done. 

I got the difference between G43.4 & G68.2 down. Now for the other stuff you explained I will probably have to read over it 10 to 20 times plus some just to wrap my mind around it. I want to say they were teaching this in one of the Emastercam lessons but I can't remember. Ron, thank you for helping me out and going in depth on how this works, I'll definitely work on it and use it.

Link to comment
Share on other sites
4 hours ago, khass0410 said:

I got the difference between G43.4 & G68.2 down. Now for the other stuff you explained I will probably have to read over it 10 to 20 times plus some just to wrap my mind around it. I want to say they were teaching this in one of the Emastercam lessons but I can't remember. Ron, thank you for helping me out and going in depth on how this works, I'll definitely work on it and use it.

My Pleasure and helps me keep it straight in my head helping others like yourself. 

Link to comment
Share on other sites
On 11/19/2019 at 1:50 PM, David Colin said:

There are some valuable info on Sandvik website about turn milling https://www.sandvik.coromant.com/en-gb/knowledge/milling/pages/turn-milling.aspx

They also have available carbide cutters with ground flat (R216.T4)

 

On 11/20/2019 at 5:00 PM, 5th Axis CGI said:

My Pleasure and helps me keep it straight in my head helping others like yourself. 

I'd like to let yall know that that endmill from Sandvik worked GREAT! The cut is super smooth, looks weird but very smooth. Thanks again.

10.jpg

11.jpg

  • Like 5
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...