Dynamic Rest Milling Issue in X6

[JMWorks]

I have a file that I am working on trying to do some rest milling from a previous operation and it keeps wanting to cut areas that are already cut and miss some that it should cut no matter how I define it, what am I missing here?

 

In the file the dynamic rest milling is Op 18 it is using a 1/2 bull end mill to come in and clean up farther what was left behind from op 14 where it used a 1.25 button cutter to high feed cut the bulk of the material out. It keeps wanting to re-cut the section with the hexagon shape and it should go around every shape cleaning up for the corner radius difference, but it misses some. The 1.25 cutter has a 13mm insert and thus a radius of roughly .255 the end mill has a .03125 corner radius so it should clean up the difference there. Both operations are set to cut 1/2" deep final and to leave .02" on walls to be cleaned up with a 1/4" bull end mill in an op I haven't done yet(was planning to use dynamic rest milling for that too). It should only clean up around the perimeter of all the shapes, the corners and inside the hook of the J shape, but it does about half of that and tries to core mill out one whole area that is already machined. I have tried several different ways to define the rest material and still don't get a desired result. Hoping someone here can shed some light on what I am doing wrong.

 

 

File is on the FTP site in the unspecified uploads folder, file name JMW_LOGO.MCX-6

[JMWorks]

55 views and not a response, I must not be the only one stumped by this...

[gcode]

just killer busy...

If someone hasn't helped you by this weekend I'll check it out

[JMWorks]

just killer busy...

If someone hasn't helped you by this weekend I'll check it out

 

 

Thanks gcode, this is a project for the company so it isn't critical but they are hounding me to get started on it this month. Still have a lot of programming left before then.

[Jeremy Herron@DBS Solutions™]

I am taking a look now. Give me minute to verify.

[BenK]

What material is it? I would use the .5 end mill at full depth and 10% radial step over instead of the 1.25 using depth cuts.

[JMWorks]

What material is it? I would use the .5 end mill at full depth and 10% radial step over instead of the 1.25 using depth cuts.

 

 

Material is 304L and each piece is roughly 11.125" x 36" so I have alot of material to remove. Was concerned with the endmill living that long, going to run it in a fadal so I am sure there will be some chatter.

[JMWorks]

Here are some screen pics

 

The OP14 roughing operation

 

Logo OP 14.bmp

 

The OP 18 rest milling operation, you can see it is trying to recut the area with the hexagon shape

 

Logo OP 18.bmp

[BenK]

My link

 

Here is a link for you to check out. Going full depth like that people are getting some great tool life. I have a few jobs that I have switched to a solid carbide tool instead of an insertable and gained tool life. The one thing to remember is to apply radial chip thinning.

[JMWorks]

My link

 

Here is a link for you to check out. Going full depth like that people are getting some great tool life. I have a few jobs that I have switched to a solid carbide tool instead of an insertable and gained tool life. The one thing to remember is to apply radial chip thinning.

 

 

I've done that quite a bit, does work pretty well. Will definitly consider that more, but I am still stuck with figuring out how I can get the dynamic rest mill to work like it should whether I cut that part with that tool path or not.

[Jeremy Herron@DBS Solutions™]

I am not disagreeing with BenK at all bcause I usually use the same approach he mentioned, but as far getting your toolpath the you wanted it, I did this and I think this is what you are after.

 

 

1: in op 18 I removed all the chains

 

2: I selected the outside rectangle as my machining region

 

3: I created a curve on the edges of the "JO" (I find soild face chaining to be buggy sometimes so I prefer to make my own geometry)

 

4: I selected the heaxagonal chain, the J, and the inside and outside of the O as avoidance regions

 

5: I set my top of at z-.490, and depth at -.5

 

6: I set the stock to leave on walls as .021 and the stock to leave on floors at .001 (if you set it at the exact amount you left it will sometimes cut areas you do not need)

 

7: regened and it looks good to me.

 

 

HTH. let me know if you have more questions.

 

[JMWorks]

Thanks for the write up jeremy, I'm away from the computer until monday now, but I'll take a look at it then.

[Jeremy Herron@DBS Solutions™]

Any time, I am uploading it to the FTP site now as JMW LOGO_2.mcx. You will probably still want to tweak the toolpath a little, but that should get you going in the right dirrection.

[Goldorak]

What material is it? I would use the .5 end mill at full depth and 10% radial step over instead of the 1.25 using depth cuts.

 

 

Material is 304L and each piece is roughly 11.125" x 36" so I have alot of material to remove. Was concerned with the endmill living that long, going to run it in a fadal so I am sure there will be some chatter.

 

 

100% agree with BenK, SS304 is a pretty easy stuff to cut , you simply need the good tooling. a variable flute high quality end mill is about 75-80$ , and you will save hours of machining using a dynamic path and full depth

[JMWorks]

Jeremy,

Just now got a look at that file, if you turn the solid into a wireframe you see that the toolpath in op 18 would actually cut off part of the solid boundary so it is still not entirely accurate, but since I have still yet to get any help from my reseller on this I am just going to program it with the 1/2" full depth and see where that gets me. Thanks for looking at it though.

[Chris Rizzo]

Hmm your running X6, and it does have much better support for bull endmills in dynamic toolpaths. Can you upload your new one and I'll take a peek.

[Jeremy Herron@DBS Solutions™]

I screwed up my chains, but it will work that way if you chain it properly and better if you split it into 2 toolpaths. I still think the 1/2 tool is a better approach fo your application though.