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:

surface finish help


GeoGirl
 Share

Recommended Posts

Hi gang,

 

Looking for a little help with surface finish. I tried to upload it to an album I created under my name, but its not working... maybe in an hour there will be 10 of the same pics in there!

 

quick description

 

aluminum part. kinda looks like the mercedes/polaris star logo. The total depth of the star is .100" and part is only 6" in dia.

 

I am roughing the part with a 3/8 ball end mill and finishing with a 1/8 ball end mill. I even switched to a different machining center to verify it was not the machine. My finishing pass is only .002" depth. I want as smooth as possible, but I am get sort of a galling or gouging effect when the shape meets the flat bottom surface. I am now running this part on a 10,000 rpm spindle. I know not much compared to what some of you guys have, but it should be able to do the job. I hope my image shows up in my album so you can see what is happening. Unless there is another way to upload a photo to this question.

 

I have tried almost all of the surface finish features, but it does not show up on the screen. I have to run it to find the problem.

Hrumph!

 

I am using Mx4 (oh I found a way to attache the file!)

 

Look forward to your help :)

 

Geo

post-14765-0-97250000-1347309384_thumb.jpg

Link to comment
Share on other sites

Try tightening up your arc filter tolerance to .0005 or less for the finish pass, and use the refine toolpath tab to fine tune. It will make it take forever to re-gen and verify, but should help with the gouging.

On your roughing paths, make sure your arc filter tolerance is half of what you are leaving for finish. If you are only leaving .002, your arc filter tolerance should be no more than .001.

Link to comment
Share on other sites

Here's how I might do it. Fill the star (suppress it if created in MC) then use the HST Spiral or SF Blend to finish the circle. Independently finish the star with SF blend, which may require several operations, or... yuck, a scallop path if you want to get it in one op. If at all possible, extend the surface edges of the star up above the circular face to use as a smooth lead in for the cutter and help to avoiding rolling over the edge and ruining the definition of the shape. Choose a blend direction that goes along the length of the points, not across. Your blend chain may look like an arrow with a point in the center of the base. (3 entities). Repeat for the other 2 legs of the star. One way cut if possible.

 

HTH, MCM

Link to comment
Share on other sites

Here's how I might do it. Fill the star (suppress it if created in MC) then use the HST Spiral or SF Blend to finish the circle. Independently finish the star with SF blend, which may require several operations, or... yuck, a scallop path if you want to get it in one op. If at all possible, extend the surface edges of the star up above the circular face to use as a smooth lead in for the cutter and help to avoiding rolling over the edge and ruining the definition of the shape. Choose a blend direction that goes along the length of the points, not across. Your blend chain may look like an arrow with a point in the center of the base. (3 entities). Repeat for the other 2 legs of the star. One way cut if possible.

 

HTH, MCM

 

wow, your explanation I think is quite over my head! :(

Link to comment
Share on other sites

Parallel is stabbing (bumping into) the edges of the circular feature. It's a easy tool path to apply almost anywhere but really isn't suited for everything. Your going to need a circular tool path to get that nice looking.

 

The blend tool path for the star only may be a bit too advanced for now. If you don't understand the suppression or surface extensions, that's fine. Use the hst spiral for better results without too much grief on your end. Cut in one direction only, don't zig zag if possible.

 

For an easy SF Blend to cover the whole part, create a circle at the outer perimeter and break it where you want the cutter to start. Put a point in the center. These 3 entities will make up the 2 blend chains required. The order and direction in which you select the chains will determine the path that the cutter takes. Yes, the point is used a chaining entity. Not hard at all. Use the spiral option. Play with along and across and 3D. This is an awesome tool path.

 

Material and cutter type / quality will dictate the feed rate.

Link to comment
Share on other sites

I would leave at least .01 material for the finish toolpath. Even with a .125 Ball Endmill, you need to have some material left over for the tool to cut.

 

Can you put a copy of your file on the FTP? Someone here I'm sure can help you with an example toolpath.

 

Personally I would use MCM's suggestion and do a blend toolpath, using a circle and a point in the center, with the spiral option turned on. I would use a tolerance of .0001, and use the filter settings to fine-tune the path.

Link to comment
Share on other sites

"Try tightening up your arc filter tolerance to .0005 or less for the finish pass, and use the refine toolpath tab to fine tune. It will make it take forever to re-gen and verify, but should help with the gouging.

On your roughing paths, make sure your arc filter tolerance is half of what you are leaving for finish. If you are only leaving .002, your arc filter tolerance should be no more than .001. "

 

 

Looks like a tolerance setting to me also!

Link to comment
Share on other sites

How do I put a copy of my file on the FTP?? Do I post my own drop site for people to access? or is there a place for that here?

 

The only reason I have been making a finishing pass of .002" is because I just try to rerun this part so I figured .002" should eliminate heavy chip loads (to rule out problem one)

 

 

 

I would leave at least .01 material for the finish toolpath. Even with a .125 Ball Endmill, you need to have some material left over for the tool to cut.

 

Can you put a copy of your file on the FTP? Someone here I'm sure can help you with an example toolpath.

 

Personally I would use MCM's suggestion and do a blend toolpath, using a circle and a point in the center, with the spiral option turned on. I would use a tolerance of .0001, and use the filter settings to fine-tune the path.

Link to comment
Share on other sites

Actually both machines are new within the last year. Both Fanuc controllers. and we are not a real production shop and these machines not used "hard".

 

 

 

Are both the machining centers you tried it on anilam crusader M's?

 

Just kidding but it isn't out of the question that 2 mills in the same shop could have similar z axis problems especially if you use them for a lot of peck drilling.

Link to comment
Share on other sites

+1 on leaving more material for the finish pass, using a different finish toolpath, and tightening up filter tolorence.

A combo of all three is needed here IMHO.

 

.002" for finish... leaving that little amount of material could be missleading. It might be that your rough toolpath is the one doing the gouging and not the finish toolpath. Can't tell by the caption though.

In addition to leaving more material for finish I'd tighten up the filter settings, as others suggested, on both the finish and the rough toolpath just to be sure. Less on the rouhg of coarse, but I always make sure it's maximum half of my stock to leave.

Nice finshes usually mean more code, so you also want to make sure you machine can keep up and not choke on the code.

Keep an eye on feed rates. Sometimes older machines will do "the robot" as I like to call it, and leave dwell marks as they pause while munching on large amounts of code.

Link to comment
Share on other sites

How do I put a copy of my file on the FTP?? Do I post my own drop site for people to access? or is there a place for that here?

 

The only reason I have been making a finishing pass of .002" is because I just try to rerun this part so I figured .002" should eliminate heavy chip loads (to rule out problem one)

 

JP's last entry in this post > http://www.emasterca...showtopic=67968

has instructions for the FTP.

 

Something is black and white wrong here. The filter setting would have to be something ridiculous to make gouges like that.... Although having more stock would be best if you are going to make more of these, the result of not having enough stock would be galling all over the floor, I don't see that. .002 should allow for a successful (not economical) "spring pass" with a 1/8" EM, if this is a one off.

Link to comment
Share on other sites

Something is black and white wrong here. The filter setting would have to be something ridiculous to make gouges like that.... Although having more stock would be best if you are going to make more of these, the result of not having enough stock would be galling all over the floor, I don't see that. .002 should allow for a successful (not economical) "spring pass" with a 1/8" EM, if this is a one off.

 

Ditto, thats why I was thinking mechanical problems

Link to comment
Share on other sites
  • 2 weeks later...

What kind of Fanuc controller is it? Does it run smoothly or jerky at the directional changes in xyz ? Could be a combo of filtering/smoothing and lack of look ahead....HPCC, AI APC, AI Contour control, etc. I wouldn't expect to see marks that big from look ahead tho.

Also if your roughing with a .375 ball and only leaving .002, that transition from .375 to .125 is awful big. I'm thinking I would do a leftover op and clear out the corners before finishing.

Link to comment
Share on other sites

Sorry for the delay all. Other jobs are a priority over this one. My controller is a Fanuc oi mc. No jerky movement with directional changes. The only reason I was using a .002" depth of cut is because I am just recutting the current part instead of making a new one every time. There should be no gouging from previous operations since I have rerun this too many times now :) I am cutting it one way and still having the same problem, but a little less. I have added a new photo and the witness line you see as a circle mid way around the star is from the tool path hitting a previous cut section.

 

This last tool path was using the advice from MotorCityMinion using the SF blend.

 

Any other suggestions are still appreciated. I should have more time this week to play with this and actually act on your advice.

 

Thanks

Geo

post-14765-0-55636100-1349300107_thumb.jpg

Link to comment
Share on other sites

I checked and my machine has look ahead (I thought so, its only a year old). I re-ran the program, just the star section and made the toolpath travel along the star and you can see in the picture what happened. Again I just reran the program .005" deeper. But I still don't believe gouging should behappening right?

post-14765-0-21705600-1349563317_thumb.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...