Help please - with Aspire modeling issue

[Ajcoholic]

I am trying to cut half-spheres out of a 1" piece of material. 12 "pockets" in a row, each 1" diameter, by 1/2" deep (a perfect half sphere)

I can model it with a 2 rail sweep or with the modeling tools (-90 degree, round shape, depth of .5").

The problem is, when I do a tool path, the upper edge of the pocket is very irregular, and rough.

Also, I would like to cut the pocket starting at the outer perimeter and cut in a circular path working deeper and towards the center, but it will only let me start in the middle and work my way out.

Help! :)

AJC

[feinddj]

try this. Strangely enough, I had just read this today.

http://fromaspiretobeyond.blogspot.com/2011/12/fixing-those-jagged-edgesthe-easy-way.html

[Brady Watson]

Hmm...I see what you mean, AJ. That is rather nasty looking even at max modelling resolution (Slowest 7x). I am not sure what is up with the toolpath either. Besides not having the ability to choose where the offset starts, the tool appears to gouge the top edge of the model - which it should not be doing.

Send a message to Vectric support. They may have run into this before, or be able to offer you a remedy.

David - I this is not normal & I don't see any way to machine between boundaries with a circle as the vector.

-B

http://i772.photobucket.com/albums/yy8/braidmeister/AspireIssue.jpg

Toolpath Sim Result:

http://i772.photobucket.com/albums/yy8/braidmeister/AspireTPResult.jpg

[tmerrill]

Hi Andrew,

If the top edge roughness you are seeing is like Brady's picture, this is easily solved by creating a flat zero thickness component. See here:

http://support.vectric.com/aspire-questions/item/why-is-machined-edge-of-recessed-model-rough

As for the direction of the finish toolpath, the Offset option always starts in the center and works outward. The only thing you have control over is the Cut Direction, Climb or Conventional.

Tim

[rcnewcomb]

In this particular case I am wondering if it wouldn't be faster and better to cut those with a 1" ballnose bit with a drilling toolpath

[Brady Watson]

In this particular case I am wondering if it wouldn't be faster and better to cut those with a 1" ballnose bit with a drilling toolpath

Definitely.

-B

[tmerrill]

Yes, that was suggested to him on the other forum he posted on.

However, knowing you should always create a zero thickness component when working with recessed shapes is important and will help him in the future I'm sure.

Tim

[mcmark]

I've run into this as well and have had good results by drawing a boundary just a couple of thousandths larger than the feature. Select your feature, then shift select boundary. This keeps the tool from going out and over the edge of the feature. You may have to adjust the proximity of the boundary to the feature for optimum results.

[Brady Watson]

However, knowing you should always create a zero thickness component when working with recessed shapes is important...

You shouldn't have to create a component with zero thickness at all...this is obscure. It should be a built-in feature that automatically & invisibly creates this 'zero thickness' component behind the scenes so that the user never has to think about.

-B

[tmerrill]

Brady,

As of now it is what it is and I'm only trying to help AJ resolve his issue and get on with his project.

I would suggest you email your suggestion to support@vectric.com so they can evaluate it.

Tim

[rcnewcomb]

I looked into this issue in this thread on the Vectric forum: ->Link (http://www.vectric.com/forum/viewtopic.php?f=28&t=6989&view=next)

[Ajcoholic]

Thanks for the replies, guys. It is 8pm here, and I was working about 12 hrs today trying to finish a cabinet job... did not get a spare minute to think about this problem.

I will read what you all suggested and try something this weekend.

I do not have a 1" ball nose bit, and dont really want to have to order one for this one job if possible. It is a job for a former employee of mine, who now owns/runs my old woodworking shop, and I'd like to get this done for him in a few days if possible.

Thanks again,
Andrew

[genek]

I dip spoons and bowls i never get that chatter at the top... I do a plunge cut to center and spiral out to the top... Could this just be chatter on the screen and not on the actually cut... Sometime the resolution on the computer can be to high..

[bob_s]

Andrew
I do a lot of pillasters with this sort of inset profiles. I use the zero plane method, as it avoids problems. There will be some ridges and grooves near the top where the profile is nearly verticle. Try and use a high reolution file and as small a step over as possible without making your cutting times too long. That is where using the large cutter really helps, no grooves and no sanding

Bob