Roughing tool path

This forum is for general discussion about Aspire

Roughing tool path

Postby ohiolyons » Wed Aug 23, 2017 2:40 pm

Can anyone explain why the roughing toolpath behaves at it does when you select a tool that has a path depth deeper than what is required? You get the error message that your pass depth exceeds what is required. You then have to play this game reducing the pass depth until it is less than required. Usually this takes several stabs to get it to work.

I'm OK with the fact that on a roughing cut it doesn't use all that is allowed. I typically pick the largest diameter to make the roughing go in the least amount of time. Larger diameter typically have greater depth of cut.

I guess I thought pass depth was a maximum, not a rule! I'm not lobbying (maybe I am) vectric to change this. I understand why not exceeding a pass depth is an important feature, but only using a portion of the pass depth, doesn't seem to be a problem.

Long story short why is this a desirable way for the roughing toolpath to work?

Thanks in advance
John
CNC in Kettering, Ohio
ohiolyons
Vectric Craftsman
 
Posts: 198
Joined: Wed May 27, 2009 7:16 pm
Location: Kettering, Ohio
Model of CNC Machine: Laguna IQ HHC, 3HP

Re: Roughing tool path

Postby Adrian » Wed Aug 23, 2017 2:48 pm

I don't do enough 3D to explain the reasoning for it when using the Z level strategy (although it is mentioned in the error message) but if you use 3D raster settings then it doesn't happen.
User avatar
Adrian
Vectric Archimage
 
Posts: 7422
Joined: Thu Nov 23, 2006 2:19 pm
Location: Surrey, UK
Model of CNC Machine: ShopBot PRS Alpha 96x48

Re: Roughing tool path

Postby mtylerfl » Wed Aug 23, 2017 3:11 pm

Hi John

That doesn't sound like normal behaviour to me. I've not gotten that message on any roughing toolpath, but maybe I'm just "lucky"! You might want to send the file along with an explanation of what you experienced, to Vectric Tech Support (support@vectric.com).

I'm interested in what they will have to say (as I'm sure you are too.) Perhaps after examining your file, they can offer a suggestion and a settings "fix" for you. I'm reluctant to blame the software until the file has been inspected for any possible errors.
Michael Tyler

carvebuddy.com

facebook.com/carvebuddy

-CarveWright CNC
-ShopBot Buddy PRSAlpha CNC
User avatar
mtylerfl
Vectric Wizard
 
Posts: 2446
Joined: Thu Jan 29, 2009 3:54 am
Location: Brunswick, GA
Model of CNC Machine: -CarveWright CNC -ShopBot Buddy PRSAlpha

Re: Roughing tool path

Postby Adrian » Wed Aug 23, 2017 3:16 pm

Michael, edit the tool so the pass depth is greater than the thickness of the model and use the Z level rather than 3D raster option. Calculate and the message will appear. The last line of the message is the pertinent one.
User avatar
Adrian
Vectric Archimage
 
Posts: 7422
Joined: Thu Nov 23, 2006 2:19 pm
Location: Surrey, UK
Model of CNC Machine: ShopBot PRS Alpha 96x48

Re: Roughing tool path

Postby mtylerfl » Wed Aug 23, 2017 3:54 pm

Ahh, thanks Adrian. Yes, I'm not too surprised the error is thrown if the Tool pass depth is greater than the total model thickness. However, it is strange the behavior isn't consistent between the raster and z-level modes.
Michael Tyler

carvebuddy.com

facebook.com/carvebuddy

-CarveWright CNC
-ShopBot Buddy PRSAlpha CNC
User avatar
mtylerfl
Vectric Wizard
 
Posts: 2446
Joined: Thu Jan 29, 2009 3:54 am
Location: Brunswick, GA
Model of CNC Machine: -CarveWright CNC -ShopBot Buddy PRSAlpha

Re: Roughing tool path

Postby LittleGreyMan » Wed Aug 23, 2017 4:02 pm

I just checked it.

The Z level roughing strategy simply doesn't make sense for me. The message is perfectly clear but I don't understand why it has been designed like this: "The depth of the Z level passes is controlled by the pass depth value for the tool".

Which means that if the path depth is greater than the thickness of the model, Aspire won't calculate the toolpath.

In the other case, it may leave much more rough material than the machining allowance. Example: 50mm thick material, 48mm heigh model, 25mm pass depth. Aspire will calculate a single pass, leaving nearly half of the raw material. Sounds perfectly illogical.

I never investigated when I got this message and simply switched to the raster strategy to get the job quickly done.

Definitely not a bug as it works as described in the dialog box, but a strange and dangerous choice if you are not watchful before running the finishing toolpath. The 8.5 manual does not describe this behavior as the dialog box does.
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: Roughing tool path

Postby ohiolyons » Wed Aug 23, 2017 4:30 pm

3D Raster solves the problem! Thanks

It happens on all files when you select Z Level, Raster X, Last is selected and the model is shallow.

I haven't tried the other options under Raster X, but i assume they will exhibit a similar behavior.

This is one of those Hmmmmgh things I would just like to understand.
John
CNC in Kettering, Ohio
ohiolyons
Vectric Craftsman
 
Posts: 198
Joined: Wed May 27, 2009 7:16 pm
Location: Kettering, Ohio
Model of CNC Machine: Laguna IQ HHC, 3HP

Re: Roughing tool path

Postby ohiolyons » Wed Aug 23, 2017 4:36 pm

just tried all options

Z Level, Raster X, First
Z Level, Raster X, Last
Z Level, Raster X, None

Z Level, Raster Y, First
Z Level, Raster Y, Last
Z Level, Raster Y, None

Doesn't matter which one you try same warning message

Guess I'm a 3D Raster man for life, now!
John
CNC in Kettering, Ohio
ohiolyons
Vectric Craftsman
 
Posts: 198
Joined: Wed May 27, 2009 7:16 pm
Location: Kettering, Ohio
Model of CNC Machine: Laguna IQ HHC, 3HP

Re: Roughing tool path

Postby ohiolyons » Wed Aug 23, 2017 4:57 pm

Just checked the manual, see below


This is my Summary of the manual on shallow models use 3D Raster on deeper ones use Z Level


Z Level Strategy

Z Level Roughing essentially uses a series of 2D Pocket toolpaths which take into account the 3D model and hog-out the material around it within the specified boundary. There are two settings that must be chosen to define this type of toolpath. The first box lets you choose the main direction of the cuts in the toolpath; either Raster X which fills each pocket with a raster pattern mainly parallel to the X axis or Raster Y which fills each pocket with a raster pattern parallel to the Y axis.

The second setting is the choice of Profile, this controls whether each level has a profile cut around its boundary or not and if so whether it cuts before the raster or after it. First does the profile before the Raster on each level, Last does the profile cut after the raster and None eliminates the Profile cut leaving only the raster pattern. These choices depend a lot on the material and tooling being used. For example, more brittle material may benefit from the profile first option to reduce chipping.

3D Raster Strategy

The 3D Raster strategy is a 3D cut which passes over the whole model. This will leave a more even amount of material for the finish cut to remove but depending on the depth and style of the part it may take significantly longer to run. In shallower parts where the roughing is only taking one or two passes then this may be a better choice. For deeper parts then typically the Z Level rouging is a more efficient. There is only one option with this strategy is to define the main cutting direction. Raster X uses a raster pattern parallel to the X axis or Raster Y uses a raster pattern parallel to the Y axis.
John
CNC in Kettering, Ohio
ohiolyons
Vectric Craftsman
 
Posts: 198
Joined: Wed May 27, 2009 7:16 pm
Location: Kettering, Ohio
Model of CNC Machine: Laguna IQ HHC, 3HP

Re: Roughing tool path

Postby dealguy11 » Wed Aug 23, 2017 6:46 pm

No reason not to use z-level even on shallower projects. Just need to reduce the depth of cut for the roughing tool and the problem goes away. I always use z-level and never had this problem until I forced it as a result of this thread.
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: Roughing tool path

Postby mtylerfl » Wed Aug 23, 2017 6:54 pm

The more I think about it, the more it makes sense that the z-level passes are directly controlled by the pass depth setting of the Tool. It does require the close attention of the user though, to avoid the error message for one, and to set a pass depth that is suitable for the particular project when using the z-level option.
Michael Tyler

carvebuddy.com

facebook.com/carvebuddy

-CarveWright CNC
-ShopBot Buddy PRSAlpha CNC
User avatar
mtylerfl
Vectric Wizard
 
Posts: 2446
Joined: Thu Jan 29, 2009 3:54 am
Location: Brunswick, GA
Model of CNC Machine: -CarveWright CNC -ShopBot Buddy PRSAlpha

Re: Roughing tool path

Postby LittleGreyMan » Sat Sep 09, 2017 11:31 am

Steve and Michael,

I strongly disagree with you -which is not my usual feeling when I read your posts :D -

This doesn't make sense for me: a roughing toolpath is supposed to get rid as quickly as possible of all unwanted rough material. So using a small depth of cut is just the opposite.

But we can't ask for Aspire's price to offer as advanced and efficient rough path as in CAM only softwares that cost more than Aspire (plus an annual fee).

Aspire offers very decent tool path for a CAD-CAM software of this price range. So it's OK while you don't have a lot of jobs which require heavy roughing.

When roughing is not too long -which is generally the case for small bas-relief- I use Aspire for the CAM part. For bigger jobs or high Z, I export the model to another CAM software.
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: Roughing tool path

Postby mtylerfl » Sat Sep 09, 2017 12:19 pm

It's certainly ok to disagree and express opinions. No problem there!

I use raster Roughing more often than z-level Roughing. It takes longer but removes more material in the nooks and crannies.

I'll use the toolpath preview and "wave" the mouse cursor around to view the various depths before making a judgement call as to which Roughing strategy will "protect" my Finishing bit (I'm paranoid about breaking bits - probably too paranoid).

Every now and then, I am surprised when I see material left behind that in my mind should have been removed by roughing. Usually play around with Tool offsets, Tool size or make new offset vectors (if using vector boundaries) until I achieve a preview that makes me all warm and fuzzy.

I've always been able to get the result I want, even if I need to experiment a little along the way.
Michael Tyler

carvebuddy.com

facebook.com/carvebuddy

-CarveWright CNC
-ShopBot Buddy PRSAlpha CNC
User avatar
mtylerfl
Vectric Wizard
 
Posts: 2446
Joined: Thu Jan 29, 2009 3:54 am
Location: Brunswick, GA
Model of CNC Machine: -CarveWright CNC -ShopBot Buddy PRSAlpha

Re: Roughing tool path

Postby IslaWW » Sat Sep 09, 2017 2:41 pm

LGM...
Right back atcha with the "strongly disagree".

The reason for this would be dense materials like local "rock hard" maple or aluminum. These of course would be on the opposite end of the spectrum from HDU sign foam. The Z level roughing, using the pass depth as the parameter that determines the "level" thickness works like a dream. Using an appropriate sized end mill with a large (~90%) stepover, a small (~15-25% of model depth) pass depth along with a .010 clearance allows you to remove material much faster that the majority of 3d type roughing toolpaths. Shallow models

The 3D finishing toolpath assumes that the bit can run at full speed, full depth over the surface of the model. In many cases using a carefully crafted Z level rough, plus full speed 3D cutting will yield the lowest start to finish cut times on models that have substantial depth in harder materials.
Gary Campbell
CNC Technology & Training
Control & ATC Retrofits
GCnC411 (at) gmail.com
User avatar
IslaWW
Vectric Wizard
 
Posts: 849
Joined: Wed Nov 21, 2007 11:42 pm
Location: Marquette, MI, USA
Model of CNC Machine: SideWinder ATC & CNC Mill on WinCNC

Re: Roughing tool path

Postby dealguy11 » Sat Sep 09, 2017 4:16 pm

Well, LGM, I guess I respect your disagreement but just as respectfully also disagree with you.

Unless you're using a truly tiny bit for carving (less than 1/16"), then my experience is that z-level roughing gets rid of enough material to allow for carving, and usually does it faster than 3d raster roughing, when you use appropriate feeds, speeds and stepovers. The "shallow" stepdown on each z-level pass is, frankly, relative and with large stepovers, as Gary recommends, irrelevant in terms of machining time.

I would be uncomfortable going the other way in most of the materials I cut -- shoving a large bit deep into a piece of hardwood. It's hard on the spindle, hard on the bit, and risks yanking the material out of whatever work holding system you're using. Granted, in a foam material this is not so much of an issue. If the carving is, in fact, shallow and I'm using a 1/16" or 1/8" tapered ballnose carving bit, I'll probably skip the roughing step anyway, and would be tempted to skip it in foam.

As I stated before, I've never before tried to shove the roughing tool deep enough in the material to get that error message. Most of the time my roughing passes take a few minutes at most. If you're uncomfortable with that, then Aspire gives you other choices.

Cheers!
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

Next

Return to Aspire - General

Who is online

Users browsing this forum: Bing [Bot] and 16 guests