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:

5 axis toolpath advice


tony1001
 Share

Recommended Posts

I have been trying different tool paths to do the channels on this part and I can't seem to come up with anything I like for it. I would like to know how some of you guys would go about doing this. The dimensions aren't critical on it and I know vibration will be an issue near the end of it, but at this point more than anything I would like to know what toolpath would work best for it. I took some details off of the part and left a parasolid with only the channels I would like to know about. What do you guys think?

Thanks

test.X_T

Link to comment
Share on other sites
2 hours ago, tony1001 said:

I have been trying different tool paths to do the channels on this part and I can't seem to come up with anything I like for it. I would like to know how some of you guys would go about doing this. The dimensions aren't critical on it and I know vibration will be an issue near the end of it, but at this point more than anything I would like to know what toolpath would work best for it. I took some details off of the part and left a parasolid with only the channels I would like to know about. What do you guys think?

Thanks

test.X_T

Impossible areas to machine on that part with bull endmills. You are correct going to require a 5 Axis machine. You can ball endmills the radius of the fillet in the floor on the channels, but cutting those with a .020 ball endmill is not going to be fun. Can rough in what you can and can finish what you can with the Bull endmill, but those transition areas on the faces from the larger to the smaller diameter cannot be cut with the same tool. A Taper Ball endmill is another choice for cutting those areas also if you can find one with a .01R and maybe a 5 ot 10 degree angle. Sometimes channel runners have a smaller radius on them. 

If you can live with a .015R Harvey offer this. 5 deg Tapered .015R Ball Endmill

I would suggest making the part long and putting a center. A Mill Turn or Tilting Head/ Rotation Table 5 axis mill would be best. Standing this thing up in the air and machining with only a .415 diameter that is over 9 x D is going to give you a fight.

Like Jparis said share the Mastercam file with your machine setup and things then someone can see about assisting.

Link to comment
Share on other sites
1 hour ago, tony1001 said:

I did what you were saying about using a bull endmill for the channels on the bigger diameter. Here is the Mastercam 2022 file. It will be for a Makino D200Z, which is a table/table machine.

test.thumb.jpg.cde2b26a5581ca1ffd42bdc0c328f82a.jpg

 

Thanks,

test.mcam

Same tool for the smaller diameter. Going to be fighting chatter on that small diameter that long, but with that machine you not given much options. I would make my own working holding and then manually rotate the part to each place I need to cut those grooves so I can support it top and bottom, not just from the bottom you would be limited to.  Yes I have made my own fixtures for index parts on 5 Axis machines.

The next question is how close does the floor need to be on the channeels to the model. Using the bull endmill will leave a cusp in the center of that channel. Only about .003 tall, but not like the diameter it is modeled to. It will be 2 flats like what you got on the bigger diameter. Where surface machining that whole channel with a ball or taper ball endmill will make it exactly like the model.

Then need to use Parallel to curve and work on those transitions.

Link to comment
Share on other sites
16 minutes ago, crazy^millman said:

Same tool for the smaller diameter. Going to be fighting chatter on that small diameter that long, but with that machine you not given much options. I would make my own working holding and then manually rotate the part to each place I need to cut those grooves so I can support it top and bottom, not just from the bottom you would be limited to.  Yes I have made my own fixtures for index parts on 5 Axis machines.

Then need to use Parallel to curve and work on those transitions.

Ok, I will try parallel to curve. The good thing is that they are mounted on 3R pallets so once I figure out how to cut one channel, I can Transform/Rotate to do the others.

Thanks for the advice.

Link to comment
Share on other sites
14 minutes ago, tony1001 said:

Ok, I will try parallel to curve. The good thing is that they are mounted on 3R pallets so once I figure out how to cut one channel, I can Transform/Rotate to do the others.

Thanks for the advice.

Tony, good luck. Might reach out to Rob at CCCS and see if he has some time to do some training with you.

Correction the difference was only .002 for the wedge create using a bull endmill to cut the channel. You can make a center cut using that surface to dirve your toolpath and then it wouldn't be so noticeable.

image.thumb.png.fdb721174bf90ae098e908596fef02f2.png

 

 

Link to comment
Share on other sites

If it absolutely needs to blend perfect, I created a floor surface along the shaft and the upper radii and lower radii, then pulled edge curves so I could create a single Coons Surface, then did a flow 5-Axis toolpath with a .015" 3fl Ball E/M. I could probably clean it up a little... did it in between somep robing stuff and a Thermal Comp test run.

image.thumb.png.6208e899064e49657e439c4c28731006.png

  • Like 2
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...