Trying to turn posts, need help on toolpaths

[John Solter]

We have a PRS Standard 96" and just recently set up the indexer. We are trying to turn the same posts that we have been running on a manual lathe, so they are just profiles rotated around the axis, nothing complex at all.

We have hit the limits of what we can do with the built in software and are experiencing both quality problems and very long runtimes.

There is no money in the budget for 3D CAM software, and since all we are intending to run are some relatively simple profiles, could someone who has better software help us out on the programming front? Or are there other inexpensive options for what we are trying to do?

Thanks.

[Brady Watson]

John,
For a job like you describe, the toolpath generated from the Tools->Indexer in SB3 that uses a profile, will do the same thing as one generated in fancy CAM software. There would be no advantage in speed or quality.

If you plan on doing mostly turnings, like a lathe, the best way to approach this would be to buy and setup a woodworking lathe, as many others have posted here. This way, you'd essentially have a 2-axis lathe that is spun independently from the ShopBot itself & tool movement could just be 2D profile cuts like you are doing now, except you'd be using the post profile shape. Spin the lathe, and do your cuts, gradually approaching outside to inside, just like a lathe.

The indexer really shines when you are indexing in discrete increments / doing non-symmetrical 3D relief type designs like 'corner' furniture legs and other complex shapes. It is meant to move incrementally, and not really spin like a lathe.

-B

[myxpykalix]

email me and I think i could help you myxpykalix@hotmail.com
send me a profile when you do so i can see what you want to do.

[John Solter]

If you plan on doing mostly turnings, like a lathe, the best way to approach this would be to buy and setup a woodworking lathe, as many others have posted here.
-B

Thank you for the advice, I should have been more specific. We would rather run the profile end to end and then turn the indexer incrementally as opposed to continually turning the post.

For the way you suggest doing it, I think building our own indexer is the best method, since running the indexer through shopbot software requires us to use their converter program. To get a .01 stepover size (which will give us the quality we are looking for), we are (according to technical support) maxing out the number of revolutions their program will allow. To avoid this, we have to use several programs to do different parts of the post.

On the speed front, the harmonic vibration from the post is causing the indexer motor to stall when we try to increase the speed above about 160 degrees per second.

[Brady Watson]

John,
There is no problem turning a post profile with the router on top of the workpiece incrementally (.01 per pass or how many degrees per pass) and just raster back & forth in X or Y using a stepper powered indexer. You could also get the profile on the front or back of the workpiece. The drawback is speed. This takes a long time to get a single finished post off of the machine & is not cost effective unless you are producing something 'fancy enough' to justify the lengthy run time.

The fastest way would be to use the Bot as a 'CNC lathe carriage' where you gradually shave down the part to the profile shape you need using your own wood lathe as a power plant. This would amount only a fraction of passes that are basically offsets of your profile - in the Z direction. You would then spin the lathe, and run each offset a stepdown distance appropriate for the material that you are cutting. This may mean shaving off only .03" per pass, until you achieve your ultimate depth of cut.

Either method can be programmed using PartWizard, PartWorks, ArtCAM or Aspire. You only need to create a 1/2 profile and position it in relation to the centerline of the material stock. There should be a tutorial or documentation for doing this in the Indexer section on the main SB site - documentation section.

-B

[khalid]

Hi Brady,
How can we generate the Lathe code from Artcam... ?.. I think you mean to create a 2D Profile toolpath?
How can we know the rotation of indexer with respect to Offset of the tool?
Regards

[blackhawk]

The fastest way would be to use the Bot as a 'CNC lathe carriage' where you gradually shave down the part to the profile shape you need using your own wood lathe as a power plant. This would amount only a fraction of passes that are basically offsets of your profile - in the Z direction. You would then spin the lathe, and run each offset a stepdown distance appropriate for the material that you are cutting. This may mean shaving off only .03" per pass, until you achieve your ultimate depth of cut.
-B

I haven't thought about this until now, but what Brady says would make turning a standard profile shape much faster. I have a standard lathe with both a stepper and the original AC motor. I can switch the belts for each off and on, so that I can spin continuously. I just can't come up with a good way to step down the Z axis as it follows a profile. I checked out the documentation page on the Shopbot website and the Shopbot Wiki but I couldn't find anything about doing this. I also couldn't find any forum posts on the subject. I think that I could get something to work out of Aspire to do this, but I would have to edit the toolpath files to take out all the extra index moves. Am I missing something simple?

For the not so good programmers like me, we need a gadget for Aspire or a Bill Young virtual tool.

[Brady Watson]

Here (http://www.shopbottools.com/files/SBDocs/SBG00139060509Indexer.pdf)- Read pages 5-7, and observe how the toolpath is offset from the profile vector. Using your noodle...Offset the original profile outwards as many times as is necessary, and toolpath each offset accordingly. BE OBSERVANT! - You will want to trim the offset vectors to the size of your stock with a straight vertical line & scissor/Trim tool in order to prevent the tool from working outside of the workpiece.

This is the same formula for ArtCAM, Aspire, PartWizard, PartWorks etc. Read the instructions in the above link on how to integrate the toolpaths you generated with the Indexer Virtual tool.

-B

[Brady Watson]

Am I missing something simple?

Who says you have to work from the Z down? Go stand on your spoilboard over the lathe...You could spin the lathe & 'profile' cut it like any other 2D shape.

-B

[myxpykalix]

Just a cursory thought...

Lets say you have a profile. You lay that out on a piece of plywood and cut it on the table in the X axis, right...

Well you should be able to use Bill Youngs utility to run the profile on the indexer. It has been so long since i used it i don't recall if it spun the indexer or just indexed it.

Why couldn't you swap Y moves for Z moves while letting the lathe spin the material. There were a couple of converters for that type of thing (I think made by Bill).

[Brady Watson]

As the saying goes, there's more than one way to skin a cat.

The simplest way to accomplish what John needs is to spin a wood lathe & do a regular old XY profile cut at fixed depth. Using the offset tool in CAD/CAM, you can offset the shape in or out and toolpath that at the same fixed depth to simulate what would be stepdown in the Z axis.

My advice would be to chuck up some styrofoam and teach yourself how to do it. You'll probably learn quickly...and will gain some useful experience - which just so happens to be the best teacher...

-B

[steve]

Here is my two cents...
Some of you guys know I do a lot of turnings on my indexer. My method has eloved to this:

turn the blank from square ( or octagon)to round. This is a seperate toolpath.
Do a Z level cut ( used rotory PP in Artcam)

Do a 3D cut with a 1/2" round nose.

For the turned sections I make a turning file using the indexer tool in SB and a modified vector made from the same vector I used to creat the 3d model. HOWEVER, I edit the file so I only use the last pass.

For any carved sections of turnings I do a 3D cut using (usually) an 1/8" tapered ballnose.

That's how I do stuff like this.

[curtiss]

As most of us do not have a 3-d Avatar,

I wondered if the Brady Watson Avatar would someday soon be available in a bobblehead ???

It would be great for the Christmas season.

thanks

[kubotaman]

Hey I really feel stupid! I have looked and for the life of me I can't find PartWizard!!! I downloaded and printed how to make a profile in PartWizard and can't find the program!? I use Aspire as much as possible, but am trying to use the ShopBot programs also, but am really failing in this area. Okay guy's where do I find PartWizad? Don't make me look too stupid okay?

[Gary Campbell]

Daryl...
PartWizard was a lowend Delcam product which used to be distibuted with a ShopBot. It has been replaced with Vectric's PartWorks. PartWorks is the ShopBot rebrand of VCarvePro. If you use Aspire, it is an upgrade of PartWorks/VCPro. Anything that can br done in VCPro/ PWks can be done in Aspire using the same directions

[kubotaman]

Thanks, I was just reading my machine instructions and just read your post. You beat me to my own answer!!! Thanks!!!