Tooling marks on straight sides

This forum is for general discussion about Aspire

Tooling marks on straight sides

Postby Henry B » Mon Sep 11, 2017 5:04 pm

Is there a strategy to avoid toolmarks on straight sides, i know from talking to a friend who uses other software that this can be avoided. Can i use another set up in toolpaths to avoid this, have had it hapoen in Aspire before, have just changed to Aspire 9 and this was the first job I tried. Thanks :)
Attachments
toolpath09.jpg
User avatar
Henry B
 
Posts: 29
Joined: Sat Nov 10, 2012 12:08 pm
Model of CNC Machine: Kimla CNC

Re: Tooling marks on straight sides

Postby mtylerfl » Mon Sep 11, 2017 6:01 pm

Are you using the Last Pass feature? Undercut the part slightly (by an amount you specify)with all passes except the last one at full depth as well as cutting it to actual size. You can even opt to reverse direction of the last pass if it helps to clean up your cut. Do a couple tests on the material you are using to see.

The software manual will explain in more detail.
Michael Tyler

carvebuddy.com

facebook.com/carvebuddy

-CarveWright CNC
-ShopBot Buddy PRSAlpha CNC
User avatar
mtylerfl
Vectric Wizard
 
Posts: 2447
Joined: Thu Jan 29, 2009 3:54 am
Location: Brunswick, GA
Model of CNC Machine: -CarveWright CNC -ShopBot Buddy PRSAlpha

Re: Tooling marks on straight sides

Postby Henry B » Mon Sep 11, 2017 6:38 pm

Hi there :)

Thanks for replying, I understand I can use profile paths make the tool bigger or smaller to cut a bit more. This is more on the inside of the M where the sides are straight, this is an imported stl file with no vector information. Its a small sample of a piece that will be 8ft in diameter when done properly and an aluminium casting will be made from my parts they will have lighting in the parts like the M that are open. I just wondered if there are better ways to set up the job in Aspire toolpathing to avoid that. It was roughed out with a 12mm tool first then a 6mm ball for finish
User avatar
Henry B
 
Posts: 29
Joined: Sat Nov 10, 2012 12:08 pm
Model of CNC Machine: Kimla CNC

Re: Tooling marks on straight sides

Postby mtylerfl » Mon Sep 11, 2017 7:41 pm

One way to clean up the internal wall is to draw a vector and run the bit (offset to suit) along the edge as a Profile. If the sides are indeed straight vertically, then use a straight (no taper) bit. If the edges are at an angle (matching a tapered bit you are using for your Finish carve), then you can use that bit for the Profile cut.

Are you finishing using a Raster or Offset? The Offset strategy has the option to run that bit (first or last) around the wall boundary automatically for you.

You mentioned other software. What does it do differently that would yield cleaner walls?
Michael Tyler

carvebuddy.com

facebook.com/carvebuddy

-CarveWright CNC
-ShopBot Buddy PRSAlpha CNC
User avatar
mtylerfl
Vectric Wizard
 
Posts: 2447
Joined: Thu Jan 29, 2009 3:54 am
Location: Brunswick, GA
Model of CNC Machine: -CarveWright CNC -ShopBot Buddy PRSAlpha

Re: Tooling marks on straight sides

Postby Henry B » Tue Sep 12, 2017 6:05 pm

Hi,

Thanks for reply, yes it was cut using offset, will experiment some more. Had the same discussion with a guy that uses artcham (had to spell wrong otherwise it replaces word with software) and he said the toolpaths strategies were much better especially on the sides of 3d objects. Will send him the file and compare abit. I really like the vectric software and have had it years now and see the improvements on each upgrade, so am not knocking things just wondered if I had missed something in toolpathing the job :)
User avatar
Henry B
 
Posts: 29
Joined: Sat Nov 10, 2012 12:08 pm
Model of CNC Machine: Kimla CNC

Re: Tooling marks on straight sides

Postby dealguy11 » Tue Sep 12, 2017 11:35 pm

Just another thought on this. When I look at the specific pattern that is carving, it looks to me as if it's coming in with the .stl file itself. The "checkering" at the top of the picture is not something I normally see when Aspire is having difficulty with straight sides.

Second thought is that if the sides are vertical, then Aspire is not going to carve them well regardless of what you do. Aspire carving toolpaths and vertical surfaces don't go together. Vertical surfaces are always cut best with 2d paths, like profiles and pockets.
Steve Godding
D&S Artistic Woodworking http://www.dsartisticwood.com
User avatar
dealguy11
Vectric Wizard
 
Posts: 1150
Joined: Tue Sep 22, 2009 9:52 pm
Location: Henryville, PA
Model of CNC Machine: Anderson Selexx 510

Re: Tooling marks on straight sides

Postby mtylerfl » Wed Sep 13, 2017 2:28 am

A little "trick" I employ with vertical sides is applying a Draft angle that matches or exceeds the angle of the tapered carving bit I'm using (thus, the sides are no longer perfectly vertical, but that's hardly noticeable in most cases).

A Draft angle is always a good idea when making a negative mold anyway. James B and I created a presentation example of "how to carve a mold" for one of the User Groups years ago. A Draft angle was essential so the rigid plastic or plaster poured into the mold wouldn't get stuck! I've never done an aluminum casting, so I don't know if a Draft is necessary or not. Maybe it would slip right out of the mold - I have no idea.

It's not "Aspire" that has a problem with vertical sides of a pixel-based model. Any software will present the same challenge when a model is pixel-based. A separate offset Profile Vector and appropriate bit selection can clean up the vertical (or angled) edge of a model, as I previously suggested.
Michael Tyler

carvebuddy.com

facebook.com/carvebuddy

-CarveWright CNC
-ShopBot Buddy PRSAlpha CNC
User avatar
mtylerfl
Vectric Wizard
 
Posts: 2447
Joined: Thu Jan 29, 2009 3:54 am
Location: Brunswick, GA
Model of CNC Machine: -CarveWright CNC -ShopBot Buddy PRSAlpha

Re: Tooling marks on straight sides

Postby mtylerfl » Wed Sep 13, 2017 4:29 am

Ah yes, another thing to consider is the resolution of the model itself and the resolution setting for your job setup. Also, the material shouldn't be excessively "oversized" bigger than the area the model covers (otherwise, you waste pixel resolution).

Are you using the new version 9? One of the under-the-hood changes is imported STL models now respect the job resolution settings whereas previously, that wasn't always the case. Of course, if the STL resolution isn't all that great to begin with, then that's a moot point.
Michael Tyler

carvebuddy.com

facebook.com/carvebuddy

-CarveWright CNC
-ShopBot Buddy PRSAlpha CNC
User avatar
mtylerfl
Vectric Wizard
 
Posts: 2447
Joined: Thu Jan 29, 2009 3:54 am
Location: Brunswick, GA
Model of CNC Machine: -CarveWright CNC -ShopBot Buddy PRSAlpha

Re: Tooling marks on straight sides

Postby LittleGreyMan » Wed Sep 13, 2017 5:48 pm

dealguy11 wrote:When I look at the specific pattern that is carving, it looks to me as if it's coming in with the .stl file itself. The "checkering" at the top of the picture is not something I normally see when Aspire is having difficulty with straight sides.


+1. Looks as an import issue.

Machining of steep walls is much better and efficient when you have a constant Z finishing toolpath. I hope we'll see this kind of toolpath in a next version of Aspire. It seems the software you mention has this feature. But IMO Aspire has other advantages, including an uncluttered UI. For artistic work, using Michael's trick is OK.
Best regards

LGM

W7 - Aspire 8.517
LittleGreyMan
Vectric Wizard
 
Posts: 416
Joined: Fri May 15, 2015 1:10 pm
Location: France
Model of CNC Machine: 3 axis Charlyrobot & Mecanumeric

Re: Tooling marks on straight sides

Postby Henry B » Fri Sep 15, 2017 8:26 pm

Thanks for taking the time to respond, have had a busy couple of days, will look at your suggestions and check how I set the job up, have also been mailed some vector files.

This is one off 22 pieces to be cast in aluminium to make an artwork in a park here that is about 8ft in diameter when put together. The M will have LED in it as will a few others, so will be cutting a 20mm 3/4"? piece of acrylic sheet to put in the hole. Will try a few things at the weekend, if I can sneak away from home.

Am on my phone now, but can do a screen capture of the stl file and toolpath settings.

Thanks again, really appreciate you taking time to help out :)
Attachments
IMG_20170915_211209.jpg
User avatar
Henry B
 
Posts: 29
Joined: Sat Nov 10, 2012 12:08 pm
Model of CNC Machine: Kimla CNC

Re: Tooling marks on straight sides

Postby honestabram » Wed Sep 27, 2017 2:14 pm

Most of the advice I had to offer has already been put out there. Not directly applicable, but if your model had been generated from vectors, one additional improvement is to make sure that you do not have excessive nodes in the vectors. I use 2-rail sweeps quite often. When you offset one vector that has bezier curves, the new vector will have a million little nodes. If you "fit curve to selected vector" or some such, it will simplify the node information and give you a cleaner model. Not helpful in your case, but just one more way to combat the really really freaking annoying fact that models are pixel based and vectors are not.

Aside from that, I've found that I get the best results on 3d modeled projects when I can go through after the finishing pass and clean up as much as I can using 2d toolpathing. When I make a column or something, I always go back and sharpen any steps with an end mill. I'd carefully trace your shape and cut just inside your model with a good end mill. I've found that a slow-spiral end mill produces an exceptionally fine edge when used as a final, offset pass.
honestabram
Vectric Apprentice
 
Posts: 11
Joined: Thu Apr 13, 2017 1:53 pm
Model of CNC Machine: Camaster Cobra 5x10 ATC


Return to Aspire - General

Who is online

Users browsing this forum: Bing [Bot], Yahoo [Bot] and 11 guests