How to make this cut as accuratly as possible.

[knight_toolworks]

I need to make this cut very accuracy and as sooth as possible. The depth will vary but most of the time it will be 1 ¼” but max once in awhile 1 ¾”
Only a ¼” bit will fit.
I planned on offsetting the cut and use a pocket cut to remove the bulk. I was thinking about .01 offset but maybe I should do more? Then make a final inside cut to smooth it up. This is cut in tropical woods purpleheart padouk ipe and such. The angle on the left is the most important to be accurate. Should it be a climb cut or a regular one for a really accurate cut.
And what bit to get the most accurate cut? Up or down cut straight flute?

7475

[paco]

I'd recommend an allowance for a final profiling at a slow rate 100% depth of cut. Is it really too small for a larger tool bit? I wouldn't suggest to stepover more than 40% of the tool bit CED, mostly for a such CED as 1/4".

Do you cut out the the part? If not, you may want to make a JIG to hold down the part at an angle to make the "pocket" along the axis rather than with diagonal moves... A JIG with two place holder will make the Bot work continuously (or almost)...

[knight_toolworks]

The cutting straight is a good idea. But I forgot that this is a mirrored part there will be another one and they will be clamped together. Of course it will be the opposite angles. Plus the parts will vary in length from 5” to 36”
But I will think about it. I had planned on using a vacuum puck to hold them in place.
There are holes and more slots to cut that I did not show. Changing the bit would be a pain on something that may take 3 minutes or so to cut total.

[richards]

Steve,
Have you thought about the possibility of using your Shopbot to cut a template and then using a hand-held router to do the actual cutting? Sometimes I get in the trap of trying to do everything with the Shopbot when I'm surrounded with other tools.

[knight_toolworks]

No it would be pointless since the way I do it now would be far better. This drawing is only part of what I am doing. Here is closer to what I am doing. These two haves have to line up perfectly.
If I can’t do it on the cnc I will do it like I have always done it. But I think the cnc will let me do things I could not do before. also the angles will vary from 45 to 60 and the lengths too.

7476

[astrat]

Steve,

Quick question .. what cad are you using ?? Is that Sketchup ?

Art

[knight_toolworks]

no this is just v care. it sucks for the job. I just drew this up as a demo. I did one accurately in part wizard. but I have a fellow helping me out with the real drawings. there are so many he can do it far faster then I can.

[Brady Watson]

Steve,
There's nothing wrong with VCarve Pro. I think it is just a matter of choosing the right strategy to get the job done. With a part like this, you really have to think a bit backwards when you create your vectors in order to create an accurate part. If I were doing it, I would create a triangular vector that extends into the waste material at least 55% of my bit diameter to avoid tool radii, like your examples above show. Then create an outside vector for the profile pass, and a couple circles for your pocketed holes.

I would do an area clear toolpath for the extended triangular part & the circles, then a profile toolpath to cut the whole thing out. Projects like these can be deceptively tricky when you know it's a simple part, but it's got you stumped. The real power of VCP can be fully realized when you learn how to use the node editing tools. You can access Node Editing mode by hovering over a selected vector line and then press the 'N' key. You will immediately have access to editing/adding/deleting nodes and spans on your vector. The angles in the example below were created by simply adding 4 nodes to a rectangle to define the end points, and then the spans in the center of the rectangle (bot & top) were deleted, giving me 2 open shapes with the angle that I wanted. The angle portions were then closed with 2 clicks of the mouse, using the Join/Close tools in VCP.

Remember...you get good at the software by playing in it, doing non-work related stuff. Don't get too frustrated, since it won't be long before you are really moving along in the software and able to create just about anything that your mind can imagine.



7477

7478


For those who are interested, CNCVideos.com will be coming out with a full training solution for VCarve Pro Autumn 2007. Another one covering Cut3D is also planned as well.

-B

[knight_toolworks]

The part won’t be cut out the two blocks of wood will be actual size. I just did the cutout to show the shape I am dealing with. I had planned on doing extended cuts though.
The problem with v carve is measuring the parts. How do you set angles when doing polygons angles and lengths? It’s not too hard in parts wizard but I don’t see how to do it in v carve. The angles need to be exact.
Another thing I find I can’t do well in v carve is merge two objects. Well you can but seldom does it come out like I want. I have more chances getting that right in parts wizard. But since you can’t export in parts wizard it can be a big pain too.
I planned on doing the area clear then the profile.
I can get these done in 3d but I figure I will get more accurate cuts doing it in 2d and I can change things around.
But myself I can’t play around just to do it. I have to have a goal. It makes practice hard but I have learned it just wastes my time.

[Brady Watson]

You can easily create a single line in VCarve and rotate it an exact angle using the Rotate tool. If you need an perfectly 90° line, just sketch a rectangle on the screen & hack away 3 legs of it. Then rotate it your exact angle. Pop in your material rectangle for reference and position the lines...It's not really that hard to do.

-B

[tmerrill]

Steve,

When I got my ShopBot over 4 years ago, all I had was PartWizard and I worked hard at learning it and getting around its limitations. I purchased VCarve Wizard as soon as the Vectric team released it and found that it did somethings excellent, but I still needed feature found only in PartWizard. Most of my projects were a combination of the two programs. As Vectric released new updates, I found myself using PartWizard less with each new release. Now, having had VCarve Pro version 4 for a day, I do not see ever needing to use PartWizard again. The program is rich with features including the ability to accuractly input lines based on specific X,Y points, angle and distance.

I know you participate in the Vectric forum, and should be aware of the new features of version 4. So my recommendation is to upgrade, spend some time with the tutorials, and I think your frustration factor will be gone.

Tim

[tony_mac]

Steve,

VCarve Pro 4.0 is being released over the weekend and you will receive the details in the next couple of days.

The release information is being sent out based on the length of time customers have owned the software, which we feel is a fair method.

We cannot release the upgrade to everyone in one go because the demand on the download servers would be too great. So we are 'staggering' the release messages > downloads otherwise the systems wouldn't cope.

*********************************************** *

Version 4 does include improved drawing tools that as Tim said, will allow you to construct the geometry required for this project.

Regards,
Tony

[harryball]

VCPro 4.0 ROCKS!

Steve, I had a very similar need to create an overlaping product from purple heart. I dialed in the accuracy over time but in the end it boiled down to taking a slow and light cut final pass, but you know all that from this thread.

In my case I also had to get the product thickness exact or the overlaps would be too high or too low. I could never get the planer set to exactly what I had last time and the small .01x variations were annoying. I finally created a custom file that measured the thickness of the material and set the cut depth on the fly.

I used VCPro 3.1 and Corel X3 to do this...

7479

7480

This is shown in the final plywood prototype before going to purpleheart. The overlap fit is PERFECT but it didn't happen in 10 minutes.

If this is similar to your need and you think it would help I'd be glad to answer the phone and discuss the challenges for a few minutes. Just send me an email and I'll give you my number if you're interested.

Robert

[srwtlc]

Not to take away from VCP in any way shape or form because it's a excellent package, but there are times that having a good cad program in your toolbox makes it easier/quicker to accurately lay out certain types of projects. Then take it into VCP.

TurboCad, AutoCad, etc., etc.

[billp]

Scott makes a great point here.
Obviously many of the programs featured here on the Forum are more CAM oriented, and in most cases they keep evolving, and improving with each successive version. But sometimes we tend to overlook the fact that there are other programs out there which are specifically targeted at performing certain functions, and their cost is negligible when compared to some of the "major" programs.
At the West Coast Jamboree some of us "reconnected"with the Turbocad line of products. They have some specific drawing programs which might help people in situations such as those pointed out lately on the Forum. One program in particular was their "Turbocad Designer (version 14)" . it costs $35 and has a LOT of drawing tools which are not in any of the other currently used software packages most people are running. It could be that many people just need something like this to "supplement"what they are now running, and then they can easily save/export their drawings to the Vectric/Delcam packages they are now using.
http://www.jr.com/JRProductPage.process?Product=4174533&JRSource=nsa &nsa=1

[tgm]

'...has a LOT of drawing tools which are not in any of the other currently used software packages...'

Could you please elaborate on this? I find it very hard to believe.

Thanks,

Tom in PA

[knight_toolworks]

Yes I have been waiting for v carves 4 as it seems it will do most of what I need. If I could export out of parts wizard life would be good. That’s been my biggest stumbling block. I like to cut in v carve if I can.
I have turbocad but it is so slow for me to draw anything it drives me nuts. It has a far larger learning curve to it.

[srwtlc]

Tom,

In TurboCad (and other cad programs) you have the ability to set up a grid on screen that will aid in drawing your object. You can make the grid as fine or as coarse as you would like. You can set it up with major and minor grid lines with hidden ones in between to keep the view easier.

Various snap modes along with that grid will aid in drawing objects precisely (along with the ability for coordinate entry too). With TurboCad, I can snap to grid, center point (arc, circle), middle, vertex, nearest, divide point, quadrant, tangent, intersection, and ortho just to name a few that I use most often.

As far as drawing tools go, you have your typical line tools, rectangles, circles, arcs, and ellipses. Then you have double lines, multi-lines, and construction lines, etc.

Then added to those, you have the modifying tools. Besides the typical weld, subtract, and overlap that are found in VCP, you have chamfer, fillet, meet two lines, split, stretch, and (the one that I wish VCP had today) trim.

Then you have all the various copy tools for liner copy, array copy, mirror (with snap points to set the mirror point), and so on.

That's just scratching the surface of what many dedicated cad programs should have in them, some may have more or less depending on what level you purchase at.

Today I have a knife box that has to have pockets at three different depths all along the same outline. I have lines that cross the main body of the outline that divide it into the three diferent areas. I can't trim those lines and create the various regions in VCP, but in TC, it takes just seconds to trim them.

[billp]

Tom,
Maybe I should have stated it to say "not in the software packages such as VCP,or PW ". Their strength is that they provide tools for both functions without having to leave the program.I think if you Google the Turbocad software you can get better details.
And of course it was just one option, there are numerous other CAD packages out there which are specifically dedicated to providing drawing tools.
Maybe I'm wrong here, but I think you'd have to spend a LOT more money to get the drawing tools in a CAD/CAM package than you can get from a dedicated CAD program. Anybody out there have any other options?

[tgm]

Bill,
You are correct. It will cost you mucho more $$ to get the combined effect of CAD/CAM together. Ask me how I know!
We still use dedicated CAD software to design and then export / import to toolpath programs of various sorts depending on the job. Some are better at the simple things. And don't let cost fool you...a simple thing like a 3D bridge in VCP, which is great due to the non-existent dwell point, is not found in CAM packages costing 10 times what VCP does.
Ask me how I know!
It's like hunting for the Holy Grail...if someone could just all the things most of us use everyday and combine them into one package, for both CAD and CAM, their market would be phemoninal...and I volunteer to be the first guinea pig.

Thanks,

Tom in PA

[knight_toolworks]

here are the first pieces. took a bit to get it right. holding down small parts is a pain. these are only 5"x3.5"
7481

7482

7483

[Brady Watson]

Vacuum...vacuum...vacuum...

I'll be doing a column very soon on vacuum hold-down for this type of scenario.

-B

[harryball]

Yes, Vacuum. Get yourself a high vac pump and make some pucks. It's not really that hard and the results are amazing. Check out...

http://www.talkshopbot.com/forum/messages/29/21297.html?1181424732

In this application I once tried to remove one of the sides after cutting with a pry bar and the vac on. I was unable to budge it with all my weight! I knew it would hold but I didn't know how well. I run a 3/8" roughing bit at 5 ips through 1.25" cedar in 2 passes. The parts don't budge.

Since it's a 3 flute up cut bit and the parts hold so well... I've been trying to screw up enough nerve to try the cut in one pass at least once to see what would happen. Haven't talked myself into it. Brady? thoughts?

This works better than I ever imagined and in retrospect I should have done it sooner. This is now my first consideration for any project I do that does not involve a full sheet hold down.

Robert

[andre]

Is it just me or is turbo cad and all cad programs difficult as heck to learn? I have turbo cad and it seems to be very complex and difficult to become proficient in. I stopped using it and I am using only part wizard now and am breezing through all my designs. I would like to go vcarve pro but they don't have simple tools like block copy and trim. I rely alot on those two functions, but I want the v-carve abilities of vcp.

[harryball]

Andre, try out the new VCarvePro 4.0 released over the weekend. It has block copy but still no trim, unless I missed it.

CAD programs can be complicated because they are designed to do so much. For the simple work we do PW and VCPro are most suited and don't have all the extra tools.

Robert

[Brady Watson]

Quote "Haven't talked myself into it. Brady? thoughts? "

What...like you need my permission to experiment??!! LOL!!! Hey, by all means, if you've got the hold, go for the gold, ya dig?


I haven't come up with a formula that completely makes sense yet in CNC land, in terms of calculating cutting force and how that relates to vacuum holding power, but the general jist boils down to surface area...yeah...yeah...we all know that part, but do we know exactly how much force on our part that YOUR particular vacuum will give you?? That my dear Sherlock, is the important question...of course without knowing the other side of the equation (or how to tell you how to calculate cutting force), we'll have utilize the tried and true MacGyver/Fred Sanford method, combining scientific formulae with shadetree common sense:

If a train leaves NYC at 12 noon and then crashes, where do they bury the survivors? Ba-dump, dump....I digress...Here we go: Let's say that I have a Fein Turbo III shopvac that realistically puts out 7 inches of mercury under full suction. Assuming that I have no leakage, the vacuum will provide a downforce of X pounds per square inch. Let's solve for X:

X = rather than go thru a whole mathematical journey, just Google (http://www.google.com): "7 inches of mercury in psi" to wind up with a value of 3.43768446 pounds per square inch, or use the chart below for quick reference:

Inches Hg--------------------------------Down-force in psi
1-----------------------------------------------0.49
2-----------------------------------------------0.98
3-----------------------------------------------1.47
4-----------------------------------------------1.96
5-----------------------------------------------2.46
6-----------------------------------------------2.95
7-----------------------------------------------3.44
8-----------------------------------------------3.93
9-----------------------------------------------4.42
10----------------------------------------------4.91
12----------------------------------------------5.89
14----------------------------------------------6.88
16----------------------------------------------7.86
18----------------------------------------------8.84
20----------------------------------------------9.82
22----------------------------------------------10.81
24----------------------------------------------11.79
26----------------------------------------------12.77
28----------------------------------------------13.75
*29--------------------------------------------14.697
* Max achievable on 3rd rock from the sun. Notice psi value is very close to atmospheric pressure, 14.7 psi

OK, so to make sense of all these numbers, let's say that we want to determine how well a 12" x 12" piece of 3/4" material will be held down using our Fein. Take the value for 7" Hg on the chart and multiply it by the X & Y dimensions. 12² = 144 square inches. Since we have determined that our Fein will put out a max hold down value of 3.4 pounds per square inch, we'll multiply to get: 144 X 3.4 = 489.60 pounds on our part...which just so happens to be a square foot or 489.60 pounds per square foot!

Sounds crazy, doesn't it? Top scientists still don't know exactly what vacuum really is, but many have simply given up, quoting 'magic' as the real secret behind this illusive technology...Seriously, we really don't fully know what vacuum really is, but more accurately vacuum simply isn't...Lost ya yet? Lemme splain: Vacuum is nothing/nothingness. It is the partial or nearly complete (depending on Hg") evacuation of atmospheric gases. The vacuum plenum that you have created for use on your CNC, evacuates the air below the entire column of air from outer space to your bleeder board, and causes the weight of this air column to press down on your material. As physics would have it, for every force, there is an equal and opposite force that opposes it. So while your little Fein is evacuating the air in the plenum, and the entire column of air from the atmosphere is bearing down on your CNC to the rate of 490 pounds per square foot, an opposite reaction is taking place below the plenum, which pushes UP to resist this force. This is why our tables don't just crush down into pile of steel, like a trash truck that fell off the roof of the Empire State Building! (imagine that if you will)

OK...so we know how to figure out how much force our vacuum will push down on the part. What's this all got to do with CNC? Well, many of us know, the hardest part of the CNC process is holding parts down. In many cases, it represents the entire 'work' portion of the job, besides swaping out material in between sipping tall glasses of pink lemonade with cherries and an umbrella sticking out the top.

While negative pressure (vacuum) is important, it is equally vital that you learn to 'think in CNC'...You must imagine and anticipate what is going to happen when your cutter plunges into the material and begins applying a lateral force to your material/part. Remember that vacuum, as it relates to a typical 3-axis CNC table, ONLY pushes in the Z direction. The router/spindle is pushing in an XY direction, putting side loads on your material, and if using an upcut spiral, you are also fighting the hold-down force of the vacuum, since it has an up-shear force to it. These factors combined can present problems if you do not have adequate vacuum pressure to overcome these forces. Additionally, CFM (airflow) plays a role here if you cut all the way through the material, exposing the vacuum chamber/plenum to the atmosphere. The more CFM you have, the better the vacuum will be able to overcome these leaks and provide negative pressure.

Here are a few things that can make all the difference in the world when using vacuum. Keep in mind that a single Fein is NOT on par with a Becker with high CFM & 25" Hg. It's OK to run a shopvac to hold down your parts, but keep in mind that you get what you pay for:

If you can get away with a straight cutter in leiu of using a spiral, do so as it will keep the z-direction cutting shear neutral. This will help reduce leakage due to up-shear forces and the material lifting & breaking the seal. Unless you are cutting out parts that are over 1.5 square feet in size and have a good vacuum system, avoid using compression spirals. They are meant to be run full depth to be efficient. They do avoid lifting the material with a z-force bias in the down direction, but put a very high side-load on the part, increasing the tendency to move in the XY. Downcut spirals are an excellent aide when cutting thin materials. Use a straight bit if you need a clean top & bottom face, or if chips are burning due to poor chip evacuation. BY ALL MEANS do multiple stepdowns when you cut your parts! I get really excellent edge quality and rarely have an issue with parts moving when I cut in 2 or 3 passes in 3/4" material. I'm never in a hurry or say to myself 'the broshure said it could cut 10 IPS at full depth in 3/4" material...YOUR machine with YOUR setup is unique & it does what it does. Focus on quality of cut 1st, then move on to the speed thing. If you are conservative AND observative while cutting with vacuum, you will learn a LOT about your particular CNC and have a better idea as to what can & can't be done using vacuum.

Here's a really trashy idea if you setup your cuts to go from one side of the table to another: Cut up the sides of a big trash bag, creating a big long sheet of plastic. As your parts are cut from left to right (make sure you order them people...I don't wanna here you got one of these stuck in your DC!)...as the parts are cut from left to right, place the trash bag over the material. Any open kerfs will suck the bag down tight and allow you to reclaim the vacuum suction that your lost by their exposure/cutting through.

As Bill P. & I said @ the Jamboree this year, there is no one-size-fits-everybody vacuum system. You have to experiement and find out what works best for you. In the next week or so, I will be posting a new column in the 'Brady's Tricks' area on how you can make a versatile vacuum jig for under $20. Regardless of whether you have a big honkin' pump, a single Fein, or just a regular ShopVac sitting around, you can get into the vacuum game, and learn how to make your vacuum setup more efficient with one of these jigs.

Til then...keep a cool tool


-B

[harryball]

According to that my smallest part once cut has about 150 to 250 lbs of down force based on my observed vac ranges. My largest part has 400 to 600 lbs (no wonder I couldn't move it) and an entire blank in place before being cut into pieces has about 1500 lbs of down force. Now, that taken with the fact that everyone knows they don't bury survivors but only make them wish they were dead after they get their medical bills... means I should probably stick with 2 passes on my smallest parts just in case but could give it a shot on the larger parts and see what happens.

Instead of the trash bag approach I've been using 3/8" tube foam weather stripping stuff. I don't know where I got it but I had 5 big rolls left after we layed the seal on the shop. It went on top of the concrete and under the seal... anyway. It works great. I can stick it to the side of a sheet and it seals or lay it on a kerf and it sucks right in. The stuff is CNC safe as it either get's pushed out of the way or cut. I've pulled it out of the DC hose many times. I'll have to post photos of it in use.

On my production files I'm very careful about cut order and so far have not had to use it on the kerfs at all. But I do seal the sides with it as I check the sheet on the initial load.

Robert

[billp]

Robert,
If it's the pink stuff they use around here it's called "Sill Seal" and it also makes great packing material when shipping jobs out to customers.....

[knight_toolworks]

I plan on going to a vac hold down once I have the time and get the details worked out. These will vary from 5” to 36” and two different widths. So once the drawings are done and I figure out the cut details then when I can find the time and the money for the parts I will set it up. I have to vacuum pumps so that parts covered.
Though if I want to cut a bunch of these at once the length of the wood could vary by quite a bit.