Spoons

[genek]

I am designing some new spoons (5 to 6) that can be cut on any shop bot with out having to have a indexer. I have run into a problem.

1. the bit plunges straight down then works it way out.
how can I have it start at the top and work down less stress on the bit.
2. after the cnc clears the bowl, the bit starts this pecking around the perimeter of the bowl.. this slows production way down. How do I do away with that pecking

[mtylerfl]

Pretty difficult to answer without a few details (a sample file would help a lot).

1) What software are you using for the layout? (Aspire?)
2) Is it a raster carve or a vector carve? If raster carving, are you performing a Roughing Toolpath before the Finishing Toolpath to avoid the bit plunging into a "bunch" of material?
3) Is it a basic two-sided machining operation?
4) Is what you are trying to carve have a lot of messy pixelation around the edges (like an imported bitmap of some kind instead of a clean model you made yourself at a high resolution? - this assumes you are running Aspire or similar software). Pixelation causes "pecking".
4b) If the recessed bowl is a negative model component that has the edge even with the top surface of the material, did you add a Zero Plane to avoid the bit-pecking around the bowl edge?
5) in your layout, have you added a recessed machining plane to allow the bit to overcarve the model but stop at a preset depth before final cutout? (again, assuming Aspire or similar software...and assuming this is a two-sided carve)

So many questions!...but we need some details to be truly helpful.

[genek]

Pretty difficult to answer without a few details (a sample file would help a lot).

1) What software are you using for the layout? (Aspire?)
2) Is it a raster carve or a vector carve? If raster carving, are you performing a Roughing Toolpath before the Finishing Toolpath to avoid the bit plunging into a "bunch" of material?
3) Is it a basic two-sided machining operation?
4) Is what you are trying to carve have a lot of messy pixelation around the edges (like an imported bitmap of some kind instead of a clean model you made yourself at a high resolution? - this assumes you are running Aspire or similar software). Pixelation causes "pecking".
5) in your layout, have you added a recessed machining plane to allow the bit to overcarve the model but stop at a preset depth before final cutout? (again, assuming Aspire or similar software...and assuming this is a two-sided carve)

So many questions!...but we need some details to be truly helpful.

1.yes using Aspire old version

2. not doing a rough not sure if it is raster or vector carve.. machine is running.
3. no it is one sided,, the way I have laid this out is to dip bowl and cut out. using sander to finish the edges.. Looks great when I did the first by hand as a prototype.

4.I used the oval tool in aspire. can't see any.
5 no. really not sure of this question

My version of Aspire is old.. Have not up-dated so that I can do designs that other with older versions can import.. this way... they can still use it if they have a newer version than I do. I wanted the newest version of aspire, but I still want to be able to meet needs of others.

[genek]

cnc just shut off.. I have it Raster and conventional. does that help.

[Brady Watson]

4b) If the recessed bowl is a negative model component that has the edge even with the top surface of the material, did you add a Zero Plane to avoid the bit-pecking around the bowl edge?


This is probably the problem. Read the help file about adding a zero plane. You'll most likely want it at the top of your model 'stack'.

-B

[mtylerfl]

Ok, thanks for the additional details. What version of Aspire are you using? I could take a look at your file, but if I made any changes, you likely wouldn't be able to open the modified file, unless I have the same older version as you. (I think the oldest version I still have is 3.5 on one of my other computers somewhere around here).

Sounds like you are rastering the spoon as a 3D carve. It also sounds like you have set your toolpath to "Offset" instead of "Raster", since it is carving "working its way out". if you set to Raster, the finish toolpath won't start in the middle of your spoon, but at one side of it. (BTW, offset and raster are both still raster carves...just a different way in which the part is tooled...round-and-round concentrically is "offset"...starting at a side edge and tooling linearly at whatever angle you choose, is "raster". I raster at 90 degrees because it is less movement for my particular machine. You have a choice to rough or not. The way you have it set up now, is the bit is plunging too deep for your finish pass. That's hard on the bit and could even break it at some point. Without seeing your actual file, it is difficult to help you further.

The Zero Plane setup is always used when you have a negative dish that starts at the top of the material...without that, you will get "chatter" around the dished edge. there is a tutorial on the Vectric website that you may want to watch for further instruction. It is the one about setting up a dished model for tooling (has a horse head model placed in a negative dish - you'll see it).

Forget about item #5, since it's just a simple one-sided job, this won't apply to you.

You can PM me if you want to arrange for me to peek at your file.

[mtylerfl]

This is probably the problem. Read the help file about adding a zero plane. You'll most likely want it at the top of your model 'stack'.

-B

Yes, he probably will, since it is an older version of Aspire. The newest version (Aspire 8) has the model ordering/dominance reversed now for that.

[genek]

Yes, he probably will, since it is an older version of Aspire. The newest version (Aspire 8) has the model ordering/dominance reversed now for that.

I went back and looked before it started the next row. I have it set for offset.. however I did not see any place that I could set up a zero plane.. I have a boundary offset which is set to zero.

will send the file tonight or tomorrow... the bed is loaded will cut till later tonight. have not gone to vetric web site yet. to read.

[genek]

i shifted to raster instead of offset.. now it is even slower.. it does 1/4 of the spoon moves to the next and so forth... what did i set wrong.

[Brady Watson]

i shifted to raster instead of offset.. now it is even slower.. it does 1/4 of the spoon moves to the next and so forth... what did i set wrong.

Many times when doing multiple parts in a single toolpath, the tool will jump around. The easiest way to avoid this is to just toolpath each individually & then save it out as a single file.

My recommendation for this project would be to get one single spoon perfected before doing a production run. It is possible to save yourself a lot of time & work later on down the line by getting the toolpaths optimized. This means running a few toolpaths & making intelligent adjustments to get it in the 'sweet spot'. Your powers of observation are key in this process.

Furthermore, there is a difference between using the one-click 'wrap vector boundary around relief' tool and manually tracing out your toolpath/profile boundary vector by hand using a polyline combined with node editing. This will result in better cut quality. If you zoom in on your boundary vector, it is probably jagged. This will telegraph into your toolpaths. Garbage in = garbage out, as they say.

It sounds to me like there are a number of little things that are fighting you. Don't underestimate the importance of reading the Aspire help file or getting some additional training. You should have received training videos as well when you purchased Aspire - it wouldn't hurt to review some of the areas where you might need some help.

-B

[mtylerfl]

i shifted to raster instead of offset.. now it is even slower.. it does 1/4 of the spoon moves to the next and so forth... what did i set wrong.

I don't think you set anything wrong. As Brady mentioned, there are strategies that can improve your toolpathing and project quality outcome. I will say that I will often use the Offset option when machining round or oval components, because it is usually faster than the Raster option (the Vectric Yo-Yo project is an example of this). However, using Offset for a recessed dish (like a spoon bowl) almost always leaves more evidence of tooling as compared to a linear Raster technique, where you would set it up for machining with the grain. (Translation...more hand sanding to get rid of the concentric tooling marks left by Offset tooling in a dish.)

I agree with Brady that investing some of your time watching the Vectric videos and checking the Help file will go a long way to helping you learn and understand the best procedures for project setups now and in the future. Also, the free Vectric/ShopBot projects use a variety of techniques that you can learn from, as well.

Your project doesn't sound complicated at all, but I fear we are making it sound like it is. It's because we have a lot more experience with the software and have run into some of the same minor issues in the past, as you are. Since we know how to avoid and/or correct them, the tendency is to spill our guts with a load of info all at once, I guess.

Seeing a file sample is still the best way to help you. At least we'll be able to eliminate the obvious (although Brady already has guessed most of the same things I have).

[genek]

Many times when doing multiple parts in a single toolpath, the tool will jump around. The easiest way to avoid this is to just toolpath each individually & then save it out as a single file.

My recommendation for this project would be to get one single spoon perfected before doing a production run. It is possible to save yourself a lot of time & work later on down the line by getting the toolpaths optimized. This means running a few toolpaths & making intelligent adjustments to get it in the 'sweet spot'. Your powers of observation are key in this process.

Furthermore, there is a difference between using the one-click 'wrap vector boundary around relief' tool and manually tracing out your toolpath/profile boundary vector by hand using a polyline combined with node editing. This will result in better cut quality. If you zoom in on your boundary vector, it is probably jagged. This will telegraph into your toolpaths. Garbage in = garbage out, as they say.

It sounds to me like there are a number of little things that are fighting you. Don't underestimate the importance of reading the Aspire help file or getting some additional training. You should have received training videos as well when you purchased Aspire - it wouldn't hurt to review some of the areas where you might need some help.

-B

Brady I learned how to do spoons when I first got the training, However I only ran three spoon profiles, and I still run those same three. ( got the cnc in 2007) Once I had the file to dip out the spoons I had no need to do any more spoons till now. I have decided to come up with some spoons that did not require a lathe or a indexer, I have forgotten how to do spoons, Plan on watching the tutorials when I get a chance... Aspire came with the cnc... Trying to rush this one spoon had a customer see the one I hand carved out, and ordered 150 of them. Before I got the cnc I did everything by hand, now I am trying to have the shop bot do all the products.

[Brady Watson]

Gene,
Everybody needs to tune up their skills from time to time - even me. So, don't take what I said as anything personal. There's lots to know and learn in this life & it isn't hard to forget or become rusty with something you haven't done in a while.

-B

[mtylerfl]

Here is a link to a two-sided Celtic Spoon project. Perhaps it will have some useful info that you can adapt for your particular project:

http://vectriclabs.blogspot.co.uk/2014/01/love-spoon.html

[genek]

Gene,
Everybody needs to tune up their skills from time to time - even me. So, don't take what I said as anything personal. There's lots to know and learn in this life & it isn't hard to forget or become rusty with something you haven't done in a while.

-B

z
Brady I don't take it personally at all.. so do no worry about kicking my rear from time to time lol...