Shallow contour depth cuts

[heilner]

Hello forum,

This is a little urgent, so I'm sorry if this question has been covered, maybe I can be pointed in the right direction quickly.

 

So I have several parts on a sheet that need various amounts of surface milling; some pieces have vertical walls and are essentially just cut out other pieces are nearly horizontal surfaces. I want to make horizontal contour passes at 1/2" depths so that the bit isn't milling too deep (the material is 1.5" thick). The problem I have is that when I set a roughing contour path and set the shallow step over it only operates on the area up until it gets to the next depth (you can see in the image that the toolpath does not mill away the material above the second and third depths, which means the bit will be milling 1" then 1.5" for the lowest path).

How do I mill away the extra stock so that all of my depth cuts are just milling 1/2"?

 

Thanks!

[Pilot Plant Supervisor]

I would use Surface High Speed Core Rough and make sure you define your stock.

[Newbeeee™]

From one Newbeeee to another

The was a thread back along where someone (sorry forgot who) posted a really good pros and cons of each toolpath. But I can't remember what the thread was called....and you think you're getting old.

Perhaps someone else can jump in with a better memory, or even better still a linky.

[Redfire427]

I think what you might be looking for is HST Optirough. It will essentially do what you have shown in your picture. You must put a value in for "step-up" so that when the tool reaches the extents of the part, the tool will "step-up" by whatever value you choose. In this case I would suggest a step-up of .1 as your depth cut is set at .5

You may also have to check the box "mill vertical walls".

 

Carmen

[Newbeeee™]

Illuminator - Here's the copy I had at work.

Really good info but sorry, can't remember who did this but big thanks to them anyway.

I know everyone here goes on about training, but a couple of booklets/pdf's like this and one describing the HS toolpaths would be excellent. It would point a lot of us in the right direction (but may do the resellers out of some training?).

Mcam Surface Toolpath Descriptions.doc

[MotorCityMinion]

1000 POSTS !!! It seemed to take forever to get here. I’ve been silent in the open forums for quite a while and was waiting for a topic worthwhile to post in. OK, so where’s my swag?

I click on the .DOC link hoping to learn something new and what do I get?

 

Here’s the link Newbeeee.

Scanning of faces - Different strategies

http://www.emastercam.com/board/index.php?showtopic=36620&hl=+great%20+chameleon#entry23894

 

How I determined the validity of those statements:

THANKS FOR THE HELP, HAPPY HOLIDAYS.

http://www.emastercam.com/board/index.php?showtopic=35674&hl=%2Bhappy+%2Bholidays

SURFACE TOOLPATH HELP.

http://www.emastercam.com/board/index.php?showtopic=37042&hl=radial#entry4170

 

Almost 2 years have gone by since those were written and with the experience I’ve gained since then I could revise those descriptions to provide a little more detail. The old school tool paths are still relevant and should be part of every programmers arsenal.

 

Lately, I’ve been using 2d peel mill and 2d blend quite a bit with excellent results by applying radial chip thinning to these strategies, cutting chains or applying them to applications that would normally be considered out of the norm or perhaps a little radical for these tool paths. IMO, keeping an open mind and not being afraid of snapping a tool or scrapping a part is the key to getting ahead here.

 

With that being said, I also apply radial chip thinning to traditional tool paths when I can and I believe we can have some fun with the part in this post.

 

This may sound nuts at first, but I would try this. Create a flat surface at your maximum depth of cut before driving through the fixture. This surface will be as large as your raw material, rectangular, plus the size of the tool we’re using width wise. In this case, let’s say a 5/8 or 1/2 ball. Lengthwise I would extend the length of the end surfaces by your raw stock. Rough the 2 ends first, 2d contour. Now create 2 chains, one at the edge of the flat surface length wise and one just across centerline by your step over amount. 10% minimum step over of the cutter diameter. Material will determine that. Use SF Parallel, chaining from the outside in (deep to shallow). If you do not have the flute length to do this, COPY your flat surface up to a plane that will work and use two tool paths, with depth limits enabled. Now repeat this for the other side. Apply the chip thinning to this tool. (http://www.emastercam.com/board/index.php?showtopic=59759). You’re going to leave a cusp equal to your ball nose radius at the bottom. Just get this with SF contour using a bull nose or indexable emill. Use depth limits and machine around the entire part to keep the tool down.

 

This sounds like a lot of malarkey so why would I do this? Well, I can get much closer to near net shape for finishing using this strategy with less air balls and I can see results in back plot that look sane, that is to say, less crazy moves that leave me wondering: WTF is this. I also don’t have access to X5 or X6 and the opti rough tool paths so a straight up comparison by me is out of the question for now. No MC installed on my home comp at the moment or I would have provided some pics.

 

If you try this strategy, let us know how it works out for you.

Hope this helps someone, MCM.

 

A tune I listen to on occasion while programming:

[Newbeeee™]

Not bad for a 1000th post

MCM. If you were a little more local, I'd buy you a pint (or three ).