Z questions..... NOOB alert

[baltic_birch]

Ok..

My stock material varies from roughly .690 to .710" thick.

Do you guys who Z at the top of material rezero for each sheet of just take a average?

I think I'll set mine to .70 in PW and try it.

I have not run any files yet..... but will there be a box to adjust the material thickness each time I run a file in case I want to run C2 for an exact match?


I guess I'm asking if I can adjust the file for each sheet if need be as I load the file. I need some dados that are exactly .25 from the top of each sheet.
Thanks for putting up with me.

[Brady Watson]

Andrew,
I take the thickest number & add .01 or .02 to it and enter that as my material thickness.

-B

[joe]

BB,

At our shop, we zero to table top allmost without exception. Not only does this eleminate problems with variations in material thickness, it also eases up the concern of material flatness.

Saves spoil boards too.

Joe
www.normansignco.com (http://www.normansignco.com)

[fleinbach]

I suppose we all have our own methods. Similar to Brady I also zero to the material top but I do not add any thickness factor. I suppose it's not as important whether you zero to the table or zero to the material top as long as you are consistent. I would think switching between the two would get confusing after a while.

[baltic_birch]

Thanks guys!

I think my routine is going to be a little bit higher than material.

I'll just run my dados on the router table. This way I'll always get the right depth no matter the thickness of my material.... plus it seem much faster than using the 1/4 endmill to clear out .7 x .25 deep.


I also do not have a vac system yet so warped sheets would require more screws or clamps to get it exact if I'm trying to dado from the top.

I've found by clamping my sheets in with a gate at one side and a clamp at the other works great. I set my profile cut to get into the spoilboard a touch and it works amazingly.... so far.

I love this thing!!!! It is wicked!!

Thanks again!



Andrew

[joe]

BB,

Please explain why would not want to controll the bottom depth of the Bit?

By estimating material thickness, and flatness with a z zero plate to the material surface, generally takes it's tole on the table top.

Joe
www.normansignco.com (http://www.normansignco.com)

Joe

[baltic_birch]

>BB,
>Please explain why would not want to controll the >bottom depth of the Bit?

I need dados cut exactly .25 in my material from its top surface.

Unless I get stock that is exact every time, how do I do that easily in a production setting?


I'm sure I'm missing something here.

PW asks for material thickness... mine changes every sheet as much as 25 thou.
The bot will not know this unless I tell it.
I can't make a part file for every specific sheet.

I have not discovered the easy way to get exact .25 dados deep in every sheet with repeating the same part file.

It is late though, it has been a long day. Maybe it will come to me in botdreams, I'm beat.


thanks

[Brady Watson]

Andrew,
You are correct. If you need precise depth dados, you will have to ZZ on top of each sheet. I never thought it was a big deal to use the Zzero plate on each sheet...It takes less than 30 seconds to do.

-B

[btk]

Andrew,
If you are doing a big production run and do not want to Z-Zero between each sheet and it appears you have a mechanism for measuring your stock thickness. If you Z-Zero to the top of the first sheet, you can then use the VA command to adjust the Z from sheet to sheet (essentially, you are re-zeroing the machine without having to use the plate each time).

After a C2 command, you are left at Z=0.5 (or some setting in your Z-Zero Routine). If your first sheet is 0.70 thick, you note that and then run your file as you would noramally run.

If the next sheet is 0.69......
you can then use the VA command to set the Z-Value to 0.51 (or 0.01 above what the current Jog Home value is). This will keep the tip of tool where it is, however it will think it is higher. In that case, when it is called to go to -0.25 (as your file is looking to do), it will go down further that before by 0.01.

There is probably a way to script the file to ask you the material thickness and then it would do the math, however the script would have to have a mechanism for storing the previous sheet thickness to do the adjustment.

Brian

[joe]

Of course Bardy is right.

The time it takes to zero isn't much of a consideration. And if your doing dado's or surface work that techniques seems logical.

I can't remember, at our shop, when a job was finished we didn't need to relieve out the part with a profile cut. There must be lots of shops who deal with more precise materials, with little no need to cut parts. A good example would be making waynescoate or 3D work.

I was talking with our old, old friend Ray Chapman the other day about HDU and it's variation in thickness. That material can be off as much as 1/8" on 1.5" in some area's. And if you zero to the top of one of these high spot, you'll be making an extra pass to cut any parts it free.

On the flat stocks such as HDU, Omega Board, etc. we leave a few thousandth on the bottom. There by keeping the whole thing together. Although this doesn't work very well with acrylic, it's a dream with PVC such as Komatex and Centra.

We all know how rough cedar varies in thickness or most any 4 quarter, 6 quarter and 8 quarter stock. Getting it to lay perfectly flat is sometimes a concern. Here is a good example for a bottom zero. Admitedly this is rather curde work compared to you finish guys.

I don't know why it took me so long to wise up to zeroing to the bed. I'm probably not alone. After all, we do call the top of the table a "Sacrifice Board".

J

[baltic_birch]

Thanks everyone.

Just to clear it up - when I zero with the plate it automatically sets this as the top of the material for my PW file. But what about the profile depth cut?

Example - I make a rectangle in PW for a profile cut. I have the model set for zero at top of material. I've put in .75 in PW for this example.

I toolpath a area clear with a finished depth of .25, a dado.

I also toolpath a profile cut to finish of .75

I save the file and toolpaths and stick the cut file on my bot pc.

I load a sheet that is only .73 thick.
I run the zeroplate routine.

I run the file.

So what happens?

I think I'll get the right dado depth.

But if the finished profile depth was .75 to begin with in PW and the top of the actual sheet was Zeroed at .73, does this mean the final profile cut is going that extra .02 into my spoil board? This would screw up and bridges, tabs, onion skins etc...

Now if I zero at the table surface in PW I can control the tabs, onion skins etc but not the dado from the top of the surface.

I can also zero the table with the plate, MZ to say .76, zero her there and use that as a pseudo top of material for PW. Or just use the the table zero as the zero point.... but that somehow got me confused in PW with cutting depths LOL. I'll go 3d that one some more.

Thanks for any further comments advice!

[bill.young]

Andrew,

If this is a production file that you will be running a lot then here are a couple more options.

If you only need to worry about a couple of possible thicknesses (maybe .72, .73, .74, .75) then you could just create a part file for each thickness upfront..it wouldn't be much more work in Part Wizard to create multiple toolpath files for different thickness materials. When you want to cut the parts you would just measure the thickness of the sheet and then run the appropriate file.

You could also modify your Part file to use variables for the various depths and then add an INPUT statement in the beginning of the file to type in the measured thickness. Then that thickness would be used to calculate the proper cutting depths, which would be placed in the variables and used in the files. It's a little more work but if this is a production file it may be worth the trouble. There's some information in the last couple of Bill's Corner articles that might help explain the process a little.

Bill

[jeffreymcgrew]

Another thing to look into is 'calibrated plywood'. Our local lumberyard brought it up to us when they found out we've got the CNC. Apparently there is plywood out there that is much more consistent in thickness and dimension, specifically for more demanding needs.

We haven't needed anything like that yet tho, so, I have no idea how much more it costs. Our supplier doesn't keep it in stock, and they keep darn near everything else, so this leads me to think that it's not common (and therefore not cheap). But you might try looking into it.

[davidallen]

BB,

Do you need a 1/4" deep dado or do you need 1/2" stock left in the board?

When I build cabinets and shelves to a precise outside dimension, it's the 1/2" left that's more important.

da

[bill.young]

I've been pushing using variables in files for a while...it really does make your part files more flexible...but know that it's pretty labor-intensive to manually convert your files to use them. To help with that I've just added a new program to ShopBot Labs called the Variablizer (I know, it's a dopey name) that automatically creates a copy of a Part Wizard toolpath file, with all the Z-axis values replaced with variables. You can pick meaningful names for each variable and also add INPUT statements if you want so that the tool operator can input things like measured material thickness...just what Andrew needs to do above. Your original file isn't changed at all so if you don't find it useful you can just delete the new file...everything's back to normal.

You can get the Variablizer in ShopBot Labs (http://www.shopbottools.com/shopbot_labs.htm)...give it a shot and let me know what you think.

Bill

[baltic_birch]

Bill, that sounds fantastic!!!


Thank you!!!

I'll get to try it in a few days.

I think I'll mic all my sheets and sharpie the value on the edge.

This will be perfect!!

Thanks!

Andrew

[bill.young]

Thanks to some great feedback from Paco there's a new version of the Variablizer in ShopBot Labs (http://www.shopbottools.com/shopbot_labs.htm) with a improved interface that's easier to use. If you downloaded it before today (1/14/07) make sure you go get the new one.

Bill