End mill profile cut out

This forum is for general discussion about Aspire
Post Reply
seabreezr
Vectric Craftsman
Posts: 105
Joined: Sun Jun 15, 2014 3:13 pm
Model of CNC Machine: CNC Shark

End mill profile cut out

Post by seabreezr »

Hi all,
I have hopefully a simple answer. I have a picture here that keeps happening. I have a cnc shark so it is a smaller one than an average owner, maybe. I do 13000 spindle speed at 100 feed rate plunge rate 30. Now this does happen with a new EM but its not as bad. I am thinking the ones I buy are just cheap. I buy from places you all do. I do appreciate this with your time spending on reading and hopefully answering as well.

Thank you all,
Happy Holidays,

Donna :roll: :lol:
Attachments
IMG_20171203_155536372.jpg

seabreezr
Vectric Craftsman
Posts: 105
Joined: Sun Jun 15, 2014 3:13 pm
Model of CNC Machine: CNC Shark

Re: End mill profile cut out

Post by seabreezr »

OH a ps. The node editing is good as well.

Bob Reda
Vectric Wizard
Posts: 858
Joined: Wed Aug 16, 2006 7:34 pm
Model of CNC Machine: shopbot 48x48 upgraded prt
Location: Monessen, Pa
Contact:

Re: End mill profile cut out

Post by Bob Reda »

slow down your speed and use a last pass cut of a few hundredths

Bob

User avatar
mtylerfl
Vectric Archimage
Posts: 5865
Joined: Thu Jan 29, 2009 3:54 am
Model of CNC Machine: -CarveWright CNC -ShopBot Buddy PRSAlpha
Location: Brunswick, GA

Re: End mill profile cut out

Post by mtylerfl »

Hi Donna,

What's the Cut quality like if you slow down the federate? From the looks of the chattered edge, you may want to run some feedrate tests quite a lot slower.

This assumes all is well with your machine (everything is tight and square) and that you have a solid and secure hold-down method for your material, collet not worn out, etc.
Michael Tyler

facebook.com/carvebuddy

-CarveWright CNC
-ShopBot Buddy PRSAlpha CNC

User avatar
martin54
Vectric Archimage
Posts: 7339
Joined: Fri Nov 09, 2012 2:12 pm
Model of CNC Machine: Gerber 48, Triac PC, Isel fixed gantry
Location: Kirkcaldy, Scotland

Re: End mill profile cut out

Post by martin54 »

Where are you buying your bits from ? Tool quality does make a difference, what does the waste cut look like ? If the quality of cut looks better on the waste than it does on the part you want then try reversing the direction of your cut.
If you are going to try slowing the feedrate & doing some testing as Michael suggests then you will need to slow your spindle speed as well :lol: :lol:

User avatar
Leo
Vectric Wizard
Posts: 4082
Joined: Sat Jul 14, 2007 3:02 am
Model of CNC Machine: 1300 x 1300 x 254 Chinese Made
Location: East Freetown, Ma.
Contact:

Re: End mill profile cut out

Post by Leo »

For one thing it is a soft wood that really doesn't give a great finish with the side cutting on the side of the wood like you are showing. You may never achieve a great cut on the same process. Maple, Cherry, Walnut should be much better.

Another thought I have is the rigidity of the machine setup. Those side cuts put a very high level of stress into the machine. The machine needs to be TIGHT.

It looks like you are taking a full depth cut. It may not seem like a lot, but for your particular machine it may be too much. Try 3-4 passes. You can adjust that in the profile cut in Vectric.

Lastly - I agree - try slowing the feedrate.
Imagine the Possibilities of a Creative mind, combined with the functionality of CNC

Oldmanofgf
Posts: 47
Joined: Tue Mar 10, 2015 11:54 pm
Model of CNC Machine: Probiotix meteor 26x50
Location: Glenns Ferry, idaho

Re: End mill profile cut out

Post by Oldmanofgf »

I agree with the other post but you might try a different type of bit your post states EM to me that says a sprail bit try a straight carbide bit one some woods I get a better cut that way but you would still need th lower the speed rate
Glenn

seabreezr
Vectric Craftsman
Posts: 105
Joined: Sun Jun 15, 2014 3:13 pm
Model of CNC Machine: CNC Shark

Re: End mill profile cut out

Post by seabreezr »

Hi All,
I do apologize for the lateness as I have been so busy but really no excuse.

I do have it cut at .125 so it goes around 6 times. I will try everything that was mentioned and keep you all posted.
I did buy from tools2day and amana bits. Sorry not sure if I can say that but I am just letting you all know where I bought my EM.

Thank you all for taking your time to respond to me and I will keep you all posted.

Happy and Safe Holidays to all,

Donna

PS. I have my boards nailed in :)

Daniel S
Vectric Craftsman
Posts: 110
Joined: Thu Jan 08, 2009 6:24 am
Model of CNC Machine: CAMaster Stinger SR-23
Location: Orange, CA

Re: End mill profile cut out

Post by Daniel S »

Hi Seabreezr,
I also have a Shark, my model is a HD4, and have experienced similar results using fast feed rates. I started with the first Shark Pro (2010) and when I decided to upgrade to a more rigid machine the sales people at New Wave Automation convinced me that this was a rigid machine and I would be happy. Well it is not as rigid as I was hoping for so since I am unable to purchase a different machine at this time I have to work with what I have. I have found that to get the results that are acceptable to me, I cut at 35 inch/min and never more then .100 depth of cut. That is cutting out projects in Alder, Cherry, Poplar, Maple and Birch ply. When I am pocketing tool path cutting I use the same numbers with no more then 25% step over to get the results. I use both Amana and Whiteside bits and get good results from both. I do not know if you use 1/4 mill up spiral or down spiral, I have found with this machine only up spiral works good. I guess the down cut must pack in the chips causing the machine to chatter. I have no problems with ball nose bits when carving 3d projects. Hope this helps, it's just my observations from my HD4 which is only 10 months old and I am still trying new things.
Dan

Post Reply