Project on tooLpath problems

[asignco]

I have a piece to make which has text on top of a rounded section. This is a true 3D piece. I cut the part into two halfs.

The problem is -I need to run a toolpath to clean up the letters. I choose a 3/16 bit and make a toolpath around the letters choosing project toolpath on 3D model. The preview shows the bit will cut deeper then the round surface in most areas. No matter what setting I choose, the bit cuts into the surface to varying degrees. The cut depth is set to zero, the bit setting in the tool dislog box doesn't seem to matter, but I set it to .125, you can't set that to zero.
I'll like to use a smaller dia bit, but I'm going too deep for most of those.
I have sent the file to vectric weeks ago at their request, but I am yet to get a response.

Is there something I'm missing? Anybody else have this aspire issue?


Thanks for any help
- mark

[RoutnAbout]

The Vectric staff usually responds pretty quick, have you checked your spam folder just incase?

I've projected onto a 3d surface several times, and haven't had any trouble.
The file to large to upload?

[gravirozo]

mark

it was discussed a few times before..
imagine, your endmill is flat on its bottom, and you sending on a path along a hillside..

the toolcenter follow the surface.. so edge will cut into the surface..

this function working well with ballendmill, or vcarving text into a surface, where slopes are not so sharp...

on the attached drawing you can see how it is occuring..

the solution for this, try to use a very small ball end mill, using 3d finish toolpathing.. like 1/32 ball endmill. around letters...
that migth helps you..

if anyway want to use the projecting toolpath option..
migth be a sharper, 15-20 deg engraving bit a very small flatend (0.015) projected to surface will help..


for other issue, with email, vectric answer for all email.. have you sent it to support at vectric?
if yes, then check your spam folder as others suggested..


best regard
viktor

[asignco]

Thanks for the response. I understand all you say. But even with a ball nose bit and a small bit there is still some cutting into the material. I once saw a video from vectric showing how to use the project toolpath function. Their video didn't shown any problems.

Thanks,
Mark

mark

it was discussed a few times before..
imagine, your endmill is flat on its bottom, and you sending on a path along a hillside..

the toolcenter follow the surface.. so edge will cut into the surface..

this function working well with ballendmill, or vcarving text into a surface, where slopes are not so sharp...

on the attached drawing you can see how it is occuring..

the solution for this, try to use a very small ball end mill, using 3d finish toolpathing.. like 1/32 ball endmill. around letters...
that migth helps you..

if anyway want to use the projecting toolpath option..
migth be a sharper, 15-20 deg engraving bit a very small flatend (0.015) projected to surface will help..


for other issue, with email, vectric answer for all email.. have you sent it to support at vectric?
if yes, then check your spam folder as others suggested..


best regard
viktor

[gravirozo]

mark

without entering an exhaustive comparison between generaly known cam programs and aspire..
shortly the two type program working differently.. what you try to perform, called pencil milling or leftover machining..
they are not offered really with aspire... some sideways are there, but not same like in camprograms..

this option basically helpful, if you want to vcarve a simple text onto a sligthly vawy surface..
the video you mentioning, i did not see.. many tutorial video still i did not see..

but heres a topic discuss this
http://www.vectric.com/forum/viewtopic. ... ing#p35932


on this topic brian gives some explanation,
also on beta forum brian or tony explained it.. migth be routenabout or some other from beta or vectric can help you more...

summarized all, still i think a small ballendmill used as finish 3d cut, limited around letters the solution for this...

if you check on that tutorial video, you will notice this method only for sligth slopes..
3d cut will not cut into surface, regardless of type of tool...

best regard
viktor

[gravirozo]

some endmills, with long or deep reach.. since you want to make only a cleaning cut, they should work for you

http://bitsbits.com/index.php?main_page ... cts_id=104

http://bitsbits.com/index.php?main_page ... cts_id=368

there are many other manufacturer producing this type of tool..

[tmerrill]

Brian explains it very well in this thread:

http://www.vectric.com/forum/viewtopic. ... 068#p73068

Tim

[asignco]

Sorry everyone, but I just did a job and ran a ball nose bit to cleanup some rough edges left by the finishing ballnose and it STILL cut into my base. I'm talking about rerunning over a FLAT surface!

Something is terribly wrong here. I had to manually change my zero point to cheat the machine in running the toolpath on a projected 3d path to get it to work!

-mark

[tmerrill]

Mark,

Without pictures and/or a file to look at, you are making it impossible for use to give you solid answers. I use zero depth toolpaths projected onto a 3d surface frequently and with the exception of sharply curved surfaces (as already explained) I get very good results.

I do have one simple question: Are you seeing this in the toolpath preview or just the machined results?

If you are not seeing it in the preview, then it is not the software and you need to look at other possibilities. You can always double check the toolpaths being created by running the .sbp file through the ShopBot previewer. This will show you exactly what cut commands are going to the controller and takes into account the post processor.

If you are seeing it in the toolpath preview, especially when projected onto a flat 3D surface, then we really need to see pictures or file to help further.

If you cannot share the entire file, can you make a simple example file that duplicates what you are seeing and post that?

Tim

[asignco]

Here are 2 files to show what's happening - the preview shows a slight cut into the surface of the recessed center area along the curved and straight path. It's most obvious as the path crosses the globe area. This recessed middle area is the same depth for all 4 sections and is a FLAT surface, yet the toolpath still cuts into the material leaving a groove along the edge as I try to cleanup the curved wall using a 1/8in in foam bit. I tried a ballnose and the result in the preview is the same. The other is a screen shot of how I set up the toolpath. If anyone can tell me if I have done something wrong in the toopath setup, please let me know. Otherwise I have not been successful using a toolpath projected on a 3D model for ANY surface flat or contoured.

-Mark

I have a piece to make which has text on top of a rounded section. This is a true 3D piece. I cut the part into two halfs.

The problem is -I need to run a toolpath to clean up the letters. I choose a 3/16 bit and make a toolpath around the letters choosing project toolpath on 3D model. The preview shows the bit will cut deeper then the round surface in most areas. No matter what setting I choose, the bit cuts into the surface to varying degrees. The cut depth is set to zero, the bit setting in the tool dislog box doesn't seem to matter, but I set it to .125, you can't set that to zero.
I'll like to use a smaller dia bit, but I'm going too deep for most of those.
I have sent the file to vectric weeks ago at their request, but I am yet to get a response.

Is there something I'm missing? Anybody else have this aspire issue?


Thanks for any help
- mark

[tmerrill]

Mark,

I am only seeing one attachment of the toolpath setup screenshot.

Tim

[tmerrill]

I am going to start with a pure guess as I don't know exactly how you modeled the logo. I did a simple example based on what I think you are describing and only covering the quadrant with the globe.

My guess is the negative Allowance Offset shown in the toolpath setup is taking the center of the bit past the 3D surface you are trying to project on. If so, Aspire will create a deeper toolpath in the center, so the part of the bit radius cutting up against the 3D surface it matched to the height of the 3D surface.

If you look at the second picture, the green toolpath is a profile inside toolpath, with -0.02" Allowance Offset, set to project onto a 3D surface which is a pie shaped flat component. The negative offset takes the center of the bit past the 3D surface, and the program calculates to keep where the bit cuts against the 3D surface equal with the height of the 3D surface.

In the third picture, I have added a positive allowance offset to bring the center of the bit inwards and ensure it is always on the 3D surface. You can see the very faint red line on the flat surface which indicates an exact depth match to the top of the flat 3D surface. Over the surface of the simulated globe shape, you can see how the bit will cut in a little more based on the effects that have already been explained. If you are trying to trim the vertical edges using this technique, just add a positive offset smaller than the radius of the bit. The smaller the positive offset, the more material will be removed from the vertical edge.

If by any chance this helps, posting your model may help us help you. The last diagram may help you see it from a side view.

Tim

[asignco]

Ok , I send the other when I get to the office tomorrow.
-mark

Mark,

I am only seeing one attachment of the toolpath setup screenshot.

Tim

[asignco]

sorry for the delay everyone - but the BMP file preview showing the toolpath cutting into the flat surface is so marginal, it cannot be seen in the preview.
but i ran the file and it happened.

i know I can always cheat by changing my z zero - but I thought this feature was suppose to work better than it does.

I'll use this method for now

Thanks for all your responses and help

-Mark