Can ShopBot do very small parts

[rkjohnson@icehouse.net]

I'm looking at the purchase of a ShopBot, but I’m not sure it can cut small pieces. Need to cut out pieces about 1”x1/2” - 3/4” thick. The laser will do this but as you know the cost is 3-4 times that of the ShopBot. How would you secure the material so the bit wouldn’t kick the part off the table? Would the vacuum system work to hold all of these parts down till the entire board was cut? Looking at 35 small parts from one board.
I live in Spokane, Wa. any ShopBots I could see operate it this area?
Thanks for any help.

[sheldon@dingwallguitars.com]

You can cut small parts with the shopbot, they are just harder to hold than large clunky parts.

Vacuum is not possible, the size of part you are talking about under perfect conditions would only have 7 lbs of atmospheric pressure on it.

If you used vacuum to hold the entire sheet and not cut all the way through would work as would mechanically holding the sheet and using tabs.

Here is a small plexiglass gear wheel done with a .025" bit. I'm sure others have done smaller things, but this job impressed the heck out of me.

87

[papadaveinwy]

Ron what sheldon is talking about is right the tabs he speaks of are small amounts of the wood not cut, this hold the part in place then when all is done you cut or snap the part out. if you draw the tab area in a differant color on your cad program then give it a depth of say -.6875 then you would leave 1/16" of material at the point of the tab then you can easily snap out the part.and just do a lite sanding.David in Wyoming P.S. to hold down the part you could use clamping or screws placed in just the right spot so the router bit would not hit them.

[rkjohnson@icehouse.net]

Thanks...I'm useing Cedar wood for this project. If I made a vacum table that only had holes under the part that was to be cut & under the remaining wood so it wouldnt move..Would that work or is wood to pouris ? I need to produce these without any additional cutting or sanding. Profit margin is small..

[windsor@muskoka.com]

Sheldon . I like the photo of the gear . ---Where did you get a .025" Bit ? Was it a 1/4" shank ? or did you have to use a collet reducer ? --or clamp a dremel tool to the z axis ?
Thanks Mike

[beacon14]

Mike;
We tried a dremel/rotozip type tool, but their tolerances are way too low for precision work like that. Porter-Cable sells a 1/8" reducer for their 1/4" collet, and many small end mills are available with 1/8" shanks
Ron;
parts that small will not be held by any vaccuum. Tell us more about what they are and we might have some other ideas. Are they rectangular, and you are doing some kind of detail on them? or are they shaped?

[gerald_d]

Ron asked, "Need to cut out pieces about 1”x1/2” - 3/4” thick. The laser will do this but as you know the cost is 3-4 times that of the ShopBot. How would you secure the material so the bit wouldn’t kick the part off the table? Would the vacuum system work to hold all of these parts down till the entire board was cut? Looking at 35 small parts from one board." To cut 3/4" deep, you will need quite a sturdy cutter (about 1/4"). If the part is only 1/2" wide, it will want to topple over - vacuum won't hold it. We would use a single "tab" in the part. In other words, do not try to cut right around, but stop short of the end.

Sheldon, was that photo before or after you changed your gearboxes to finer ratios? In general, what is your experience of changing the gears to improve cut quality? (I hope that my memory serves me right, and that you did in fact change your ratios........)

[mikejohn]

This thread flowed over from the newbee thread, and answers perfectly my main concern for my use of the SB.
Am I correct in believing that if a sufficient amount of tab is left in place to prevent the piece moving, then very small pieces can be cut?
The gear part of the gear wheel looks very small. Each tooth appears to be about 2.5mm long. Is this about right,Sheldon?

[sheldon@dingwallguitars.com]

Mike, I got the bit from Think and Tinker (www.thinktink.com), KBC, MSC, Robb Jack all have them. I like Think and Tinker for the customer service.

The spindle was made by Air Turbine Tools. The spindle runout tolerances are extremely tight. Which is what you need when using small bits. .010" of runnout is almost 1/2 the diameter of a .025" bit.

Gerald, this was done after upgrading the controller and steppers for about a .001" step resolution (I can't remember the exact amount). Cut quality did indeed improve to the point where I'm as satisfied as I can afford
We do alot of curves and extremely shallow angles. This is where I noticed the improved quality - YMMV. I wonder if it would be possible to temporarily "jury rig" the shopbot to do finer detail, by changing the unit values and correspondingly scale up the drawing?

Mike, the teeth are 1.34mm long, the OD of the gear is 6.44mm. The part replaces one set of planetary gears in a Black and Decker cordless screw driver. Taking the RPM from 180 to about 1600. The tool now makes a great little string winder.

[gerald_d]

Sheldon, the jury rig you speak of, is exactly what us metric guys are doing - we have 25.4mm to each of your inches and we get exactly the same qualities as you (before you changed the gears)

Mike, this is our approach for cutting small parts in hardwood - with firstly some examples of what NOT to do! The 12 blue circles are the finished parts that we want out of the board, with the grain direction shown in yellow.


88

We can clamp the board to the table with two G-clamps and proceed to cut circle no. 1. We plunge at the 3 o'clock position and go clockwise around back to the 3 o'clock position. Problem A - no tab and the part flies out. Solution A - Stop cut at 12 minutes past and this leaves a small tab.


89

Problem B. The grain of the wood tears into the part as we try and break off the tab. Solution B. Position the tab at where the grain is tangential to the cutting direction (6 o'clock or 12 o'clock)

So we change the plunge/tab/start-stop position to 6 o'clock and then happily proceed to cut parts 2 and 3. Part 4 starts nicely, but when the cut reaches about 9 o'clock on part 4, DISASTER STRIKES!


90

The left hand clamp has been cut free from the workpiece and the right hand clamp alone is not enough to stop the workpiece from shifting! Problem C. Clamps are rendered ineffective. Solution C. Start the cuts furthest away from the clamps. Like this:


91

We always start furthest away from the 0,0 reference point. A huge advantage of this is that we keep the file of the board that has not been cut yet (offcut). We therefore have files of all of our "off-cuts" and can very quickly reposition them at 0,0 for a next client/shape. In this example we would cut in the sequence 11, 8, 10,12, 5, 6, 7, 2, 3. Always making sure that there is a firm "base between the clamps.


92

The cutting of parts 4 & 9 can present us with the same problems of clamping again. In this case we would either move the right side clamp, or add a third clamp.


93

[mikejohn]

Gerald, like all things computing, obvious once you,ve done it, a complete mystery when you start. It took me 20 minutes to find how to change from imperial to metric units in the preview programme!!
If I can repeat myself, it appears the Shopbot is very capable, we just have to learn it's capabilities, and this forum is the greatest learning school ever.
Mike

[gerald_d]

Mike, if you followed my logic carefully above, can you tell me where the tabs should be in each of parts 1, 4, and 9 so that the two clamps are enough? (The 6 o'clock position is not the best for these 3 parts). Surely, for this to be the greatest learning school ever, you do expect to write a test?

[mikejohn]

That made me read it all again very carefully!
The logic, I think, requires the tab to be close to the clamping position. This would be at 4 o'clock for 1, 8 o'clock for 9. Cut these 2 first. Then to cut 4 at 4 or 8 o'clock. I realise the cross grain snap off remains a problem but I presume you would cut the tabs off.

The beauty of learning via these forums is, a question is posed, you can puzzle over it waiting for the replies, and when thy come, find theres more than 1 solution. Add your own ideas to these, and you understand more of what you're trying to learn.
However, I welcome the ideas of direct questions.
It forces you not only to read the answers, but also to try hard to understand them.
I am really impressed with Sheldons gear wheel.

[gerald_d]

Mike, I was being nasty to you to put you under pressure like that - but you scored 100%!


The messages that I am trying to get across are:

- One can hold parts with simple clamps if the job is planned carefully.

- It is often better to insert "tabs" manually, rather than let the SB do it automatically.

- The cutting direction (clockwise/anticlockwise) is relevant when planning a job

- grain direction is relevant.

- sequence of cutting parts is relevant.

- the actual size of the part is only relevant if you want to try and hold small parts with vacuum, but mostly the use of vacuum can be avoided.

You being a proficient AutoCAD man, it may be interesting to you that we do that the whole process described above in AutoCAD. Every single move of the tool is represented by a line in x,y and z coordinates.

This is a "plan" view and "isometric" view of the job before we ask the CAM program to write the code for us:


94

95

(Notice the extra height in some places to pass over the clamps)

When we go to this level of detail in AutoCAD, then it is only 4 or 5 clicks in Vector (and hopefully also in Parts Wizard) to write the DOS file. People who are less proficient in the CAD side, would expect the CAM side to do more for them. We maybe go overboard with the AutoCAD, but that is why we so confidently predict the SB's movements without previews and test cuts.

[mikejohn]

All is becoming clearer.
Make your drawing in AutoCad, but include x, y AND Z. Use a continuouse line for cutting, including the first Z down, then the Z up and jogging in a dotted line. I presume the direction of drawing is also the direction of cutting. Do you assign the type of line used in Autocad for cutting or jogging, or is there a SB default?
I admit to have been a little worried a few days ago, reading some of the older forum messages, but most of the dificulties experienced seem to be answered succesfully by others.
Send more posers, it really makes you think!
Mike

[gerald_d]

Mike, you must have noticed the deathly silence from all of the other ShopBotters, because I am probably talking Greek as far as they are concerned!


My impression is that most SB'ers do NOT go to this level of detail with their programming - I do it because I can, and I think you can too (being an AutoCAD 3D survey man). But, I don't want to lead you too far down the garden path. In any case, you will probably get Parts Wizard, a program that I am not familiar with. Already, the solid versus dashed lines in my example are required by Vector to indicate the different speeds - PW may require another system of line/speed differentiation.

There isn't a single "right way" to do the programming. But you can use your existing skills to the max before feeling obliged to learn a lot of new stuff.

If I made a dxf of the above AutoCAD file and fed it directly into SB's DXF converter, then we get a strange result: Each line segment is cut in the same sequence and direction in which it was drawn. Imagine the disaster if all the cirles were cut first, then all the verticals and then all the transits above the surface!

This is where the CAM program comes in. We give this dxf to Vector (or other CAM capable program) and look at the iso view (like above). Then we click on the point where the tool must start and tell it to run to the end of that line segment and look for an attached line segment. (we can say that 0.01mm is considered as attached). And so it carries on right to the end - giving our sequence and direction. And it writes the "DOS" code for all of this!

You will see a couple of methods described on this board of how to tackle the sequence/direction "problem" - most of them rely on non-CAM methods, because "CAM was too difficult to learn". My take on this is that the CAM programs are loaded with too many bells and whistles for the guys who are already familiar with some form of CAD program.

Mike, my advice to you in your particular situation, is to concentrate on how you are going to determine sequence/direction after you have done a good .dxf. If you have already paid your money, you can ask SB to ship your CAM program early (if they have not already done so - check those CD's carefully!)

And, apologies to Ron who started this thread on small parts, I have gone way off the topic!

[mikejohn]

Ron said " but I’m not sure it can cut small pieces."
I think your example, and your explanation is still on topic. It seems to me the SB can do anything, (even make the coffee!), if you know whats needed from the software, and from material handling.

[papadaveinwy]

Mike and Gerald, I fully understand the line of thinking you are following and I believe you would be supprised at the amount of botters that do follow it. As with other threads when someone is taking the right route then you may notice that not alot of imput is put in, but I would recomend that in 3/4" material that at the point of tabs you would draw those points at a different depth color so that it will facilitate ease of seperation.As in my post above if you route those at -.6875 eventhough the sections become loose from the clamping area then the remaining wood on each section will be easier to break off and could be cleaned even with a razor knife or as I said a little sanding. you could accomplish this by changing color at the tab point and continue to draw the design till just befor the point of contact to the other side of the circle then do your zup line and your segmented travel line. if you kept this portion of the tab to a tollerance of say 1/64" then it would still stay conected to the larger portion. just my peabrain thought. David in Wyoming

[pcampbell86@charter.net]

hello People

Just a thought..i think you would be very surprised if you knew just how many people were reading these posts of information..
when you guys give such valuable info to us all we just sit back and read it and learn

why mess with a good thing by sticking our noses in..like i just did now lol..keep it up fellas its great

[rkjohnson@icehouse.net]

Gerald
Thanks..the steps will solve the problem on how to deal with small parts. It looks like I will just have to do some trim work. The only way out is with a laser, which I cant afford.
Thanks to all of you that responded. The only thing I need now is for SB to lower the price so I can purchase one.

[gerald_d]

Yes David, with very hard or thick material, we do trim down the thickness of the tab part. Generally, they will be multi-pass cuts for our little router in any case, so we only put a tab in the last pass.

But there are also times when we ditch the tabs and just follow the SB with a hold-down stick - for very soft and thin parts, if there are not too many.

Other times, we pick a board that is slightly too thick, deep-engrave the parts into it, and then use a thickness planer to skim off the back and release the parts. (for longer parts that won't jam up the planer).

And then there are adhesives, wedges, vacuum, . . . . . . . all of them already discussed all over this Forum


Our first choice for holding the work is always g-clamps and we take it from there.

[srwtlc]

Ron,

On the subject of holding your small parts, I've had several jobs that required cutting many small parts out of a blank of material. What has worked well for me has been to make a dedicated vacuum jig made from 1/2" MDF and using a 6hp ShopVac that holds the blank down. Some of the jigs also have a raised edge that helps to keep the blank from sliding either direction. Although my blanks were of 1/8" and not 3/4" material, you could probably get away with the same method. Although you will have to use tabs and sand them off with say a stationary edge or disc sander (pretty quick work). The idea here is to utilize the surface area of many to hold the whole.

My method...First make the jig out of two layers of 1/2" MDF. The top layer has the holes under your parts plus any area outside the part that can be used, just not an area under the actual toolpath. The bottom layer is the manifold that connects all those holes. And provide a port for the vacuum hose (I usally make an extended portion of both layers with a hole to fit the hose on the top layer and a smaller hole in the bottom layer to stop the hose from sucking down into the bottom layer) Then sandwhich/seal that all together. Attach some edging around the outside to make a lip to keep the blank from sliding back and forth. You will need to plan your toolpath first as that will determine how the holes will be for your vacuum surface. The use of vacuum, an edge lip, and a downcut spiral bit may be redundant, but if you need to do these on a consistant basis (production runs) it works pretty good. Just index it on your table and zero off the corner of it.
As far as your toolpath goes not only will you need tabs at the ends of your 1" pieces, but you may need to leave some webbing between the rows or tab the sides to keep the rows from vibrating. Your cutting sequence will determine some of that. You will have to end each pass going with the grain though or you'll have blowout on the ends.
I've done thousands of 1/2" x 3" canoe paddle keytags out of 1/8" baltic birch for a local brewery this way and it works great.
Now that I think about it, wouldn't it be easier and less waste to rip these strips on the tablesaw and crosscut them with a mitersaw with a zero clearance fence? Yea, I know, but its more fun on a ShopBot! ;-)

Gerald,

I'm one of those guys that goes to the level of detail as you do. I'll draw up the majority of my parts in TurboCad and take them into Vector for the rest, unless if the part is fairly simple then I'll draw it in Vector too. I don't bother with the ups and downs (connect to Z) though, I make Vector handle that. When I first got my machine and Vector with it I used to get so disgusted with it (Vector) that I wanted to rip it out of the computer by its .dll's. I have stuck with it though and have found it to be an invaluable tool. I've tried some other Cam programs and find all the extra dialog boxes and tool inventories to be annoying. I know I'm going to use this or that bit, so I know I'm going to need this or that offset and just give me the code already will ya. That's the simplicty of it. For some of my parts I can't imagine having to draw everything in succesive order to be able to get the right sequence from a converter produced code.

Anyway, thats just one mans opinion. (As he steps down off his soapbox, picks it up, smiles and walks off)

Scott

[gerald_d]

"wanted to rip it out of the computer by its .dll's"



I think that I have found a kindred spirit in Scott! Our love/hate relationship with Vector is the same as yours!

(PS, we normally also use the "connect at Z", but I wanted to show Mike that this type of thing can be done with his existing 3D CAD program.)

[mikejohn]

Gerald, reviewing your drawings showing the order of cutting, it occurs to me that when, for instance, you have cut to 12, then 11 is now free, as also is some offcut pieces. Do you lift these clear whilst you are still cutting, or is it safer to leave this until the SB stops?
Mike

[gerald_d]

Generally, if we have to "nest" very tightly and have cutting paths overlapping with loose offcuts, we use a stick (or air gun) to move away the off-cuts during the cutting. We very seldom let the SB cut unattended. Unattended cutting is only considered where we know that NOTHING will be loose after cutting. For cheaper MDF, we do not nest so tightly and leave a "border" around each part.

To be frank, the actual risk of injury is not the major concern. A flying chunk of work can break the expensive bit. Or it jams the bit and forces the workpiece out of position, causing incorrect cutting from that point on.

[sheldon@dingwallguitars.com]

Like Gerald, I use AutoCAD to generate the drawing. In Gerald's example (and I realize he is just showing one way of doing things) I would have to do the Z movements in Vector because my version of AutoCAD (LT) is 2D only.

I find the Function Arrow in Vector really useful. With it, you can manually move the start and finish points of a circle or line quickly, placing the tab anywhere you feel like or adjusting the size of the tab.

Another cool feature is while your tool path is selected, you can go to attributes and adjust the line width to the size of your cutter, then de-select the tool path to get a visual of what the tab will look like when cut. Often times, especially on small parts, a tab will look adequate when drawn, but turn out to be too small once cut if I don't do a visual check first. There are other ways of doing this, but for me this works.

[gerald_d]

Sheldon, for many years I also believed that AutoCAD LT is 2D only - till somebody showed me that it is capable of 3D "wireframes". I use LT2000 now, and I don't know if the 3D only came with later versions of LT. If you look at the "Properties" of a line, does it tell you the x,y,z coords of the ends, or does it only tell you x,y? (That question was my intro to the 3D capability).

As a general rule, I make the "tab" break in the line equal to 2xBit Diam. and adjust from there. Nice to see another closet Vector supporter!

[mikejohn]

Slightly off topic, but.......
Using a very small pointed bit, how small do you think you could engrave SHOPBOT around 1mm deep in softwood?

[gerald_d]

The coin is 19mm in diameter. Notice that the font of the letters has been discerned by a varying depth of the V-cutter (from 0 to 1.2mm deep).


96


These strips of plastic were 8.7mm wide and the writing was a fixed 0.3mm deep:


97

[sheldon@dingwallguitars.com]

Gerald - you've just saved me day's of work trying to find a fix for some arcs that were somehow misplaced in Z on my master drawings. I've been putting off dealing with this for years because I couldn't find a simple solution. I'm going to look into the logistics of shipping a case of Canadian beer to SA - thanks.

Regarding the font with the variable Z depth, did you manually program that, or use SW? I have a logo project that requires arcing Z depths to duplicate the look of a hand brushed script.

[rkjohnson@icehouse.net]

What is the smallest diameter bit you can use to cut 3/4" soft wood with the SB?

[gerald_d]

Hi Sheldon, which version of LT have just discovered to be 3D-capable?


We have VCarvZ for the variable depth programming - mail me your traced logo (dxf) and we'll take a stab at it.

[rgbrown@itexas.net]

"What is the smallest diameter bit you can use to cut 3/4" soft wood with the SB?"

The limiting factor will be the bit (IMO). One of my "general" catalogs lists a 3/32 carbide bit with a 3/4" cutting length, spiral upcut.

Ron

[gerald_d]

The smallest diameter bit question is tricky . . . . . .

For production work at a reasonable rate of cutting, I would say a 1/4" bit. But if you want to experiment, break a bit or two, it depends on whether you could buy a smaller long bit - like Ron Brown said. You can set the SB to move very slowly and smoothly and so you can break less bits than with a hand-held router. But, do you have that patience........?

[rgbrown@itexas.net]

But, do you have that patience........?

And, many other variables - like can you clear the chips, how much depth per pass, spindle speed....

I have seen the "rotozip" bits ~3mm spiral down, This would mean the material would need to be elevated and the chips would go below the part and create another batch of situations to correct.

[mikejohn]

This is an old thread, but I have a question about tabbing.
If I am cutting small parts, between 25mm (1 inch) and 100mm (4 inch) diameter (or square), should the tab be opposite the cutting start point?
That is two opposite sides of the piece would be held right up to the last moment, surely eliminating any possible movement of the piece. Or doesn't it matter if the tab is only 1 cm (1/2 inch) from the 'breakthrough' point?
Mike

[notsure about runnout (Unregistered Guest)]

How is runnout measured? Is your value what runnout on the part is at it's worst or is it added up somehow?

[mrdovey]

I just noticed the "smallest diameter" question; and thought I'd chime in with the info that this past week I was routing in pine with a 1/32" up spiral. I think I'll have to get a 1/64" bit just to try it out...

[mikejohn]

Morris
how thick was the pine?
What speeds were you cutting at?
.........Mike

[rookie432]

O.K. I want to know where to get a 1/32" up spiral bit???

Oh and what Mike said too

[paco]

www.harveytool.com (http://www.harveytool.com)

www.bitsbits.com (http://www.bitsbits.com)

[mrdovey]

Mike, the pine was a 1x4 (0.75" x 3.5" or 19mm x 88.9mm) and I cut 1/8" deep in four 1/32"-deep passes.

Spindle speed was 18,000 RPM, feed speed was 1.375"/sec and the xy ramp rate was set to 0.5 (because there were a lot of sharp angles and because I only have two of the bits.)

You might find it interesting that I've yet to break one of these little things (I only break larger bits. )-:

Bill, these came from http://www.precisecut.com/
Another source is: http://www.hartlauer-bits.com/