Tool change

[WoodMizer]

Wondering if any one out there can give me a hand.

I'm making a woodworking project and I'm trying to set up my machine so that I can drill pilot screw holes with a 1/8 tool and then switch the tool to a 3/8 compression bit to cut out the piece.

Just wondering how I do this in lazycam and/or Mach3. It looks like there are multiple ways to set it but so far it doesn't seem to be recognizing anything.

I would need to tell the machine what tool I want to use on a specific chain, to pause so I could change the tool in the spindle, and then restart with the new tool.

At the moment I think the machine is not recognizing the 1/8 tool diameter and is cutting a circle instead of a straight plunge for a 1/8 hole.

Any help would be greatly appreciated. I've looked at some of the tutorial videos on ArtSoft.com and it doesn't show much or I just can't find it.

Thanks,

WM.

Similar Threads:

• How to change Tool change position(About MAZATROL T1 control)
• How do I change the Tool Change Position?
• Need Help!- Bridgeport interact 412 tool changer does not slow b4 tool change
• Auto Tool Zero Sensor & Connection Checker, Cnc, Tool Change / Measurement.
• need help wana make macro for getting tool change by giving tool pot no on vmc instea

[SORCHEROR]

in the mach setup did you check to see if you have ignore tool change turned on,might be the problem

[WoodMizer]

Thanks. I'll give that a try.

I'm still not sure if I'm doing anything right. Do I manually put the tool change into the G-code? Can I assign different tools for different chains? Is this all done in lazycam or can I set things in Mastercam?

[ger21]

I don't believe you can post code for multiple tool sizes in LazyCAM. You'll need to create the g-code for the 1/8"tool first, then separate code for the compression bit.

Or use a different CAM package that can output code for multiple tools and operations, like Vectric's V-Carve pro.

Typically, when you have a tool change, you insert an M6 in your g-code, like this:

M6 T2

This will have Mach3 change to tool #2.

There are 3 different ways to set up Mach3 to handle M6's.
First, is ignore them, which you probably don't want.

Second, is "Stop Spindle, Wait for Cycle Start". This will run the M6Start macro, then stop and wait for you to change the tool. Then, you'll click Cycle Start, which cause mach3 to run the M6End Macro, and proceed to cut.

This is the standard method, if you do not have an automatic toolchanger.

I believe the default M6 macros, just move the tool to the toolchange position, and return it back before proceeding.
I use modified macros that zero the tool after changing it. You'll need to zero the new tool prior to cutting with it.

The third M6 option is for those with fully automatic tool changers.

[WoodMizer]

So, if I'm trying to make a cabinet with pilot holes I would.....

Load my DFX file into lazycam. Delete the chains that contained the panel cuts (3/8" compression) so that I'm left with the holes (1/8" tool). Post code for the holes and then do it again for the outside cuts (without the holes)?

How do I make sure the holes end up in the right place?

How does MasterCam know about the two different tools? Can I just put in an M6 with Tool #2 and have it figure it out from Lazycam (since the tool is set up in lazy cam)?

And, telling lazycam (when I set up tool #1) that the the pilot hole tool is .125 (1/8") it always changes it back to 4.000 "units" and cuts circles instead of just a hole.

As I've said before I only do this sporadically between jobs and don't really have any official training except for a course in SolidWorks so I really thank you for all of your help.

[ger21]

How do I make sure the holes end up in the right place?

I don't use LazyCAM, but you'll need to set the origin to the same position.

Not sure how MasterCAM is involved here??

You might want to spend some time reading the LazyCAM manual.

LazyCAM

[WoodMizer]

Sorry, I also have a copy of Mastercam that I haven't even tried to figure out yet. Maybe it would work better?

[WoodMizer]

Sweet, I didn't know they had a printed manual. I thought it was only the on-line tutorials. I don't have the intermatron in my shop which makes this whole process even harder. Trying to remember everything fromt he 1/2 hour video and then trying to recreateit later in the shop is hopeless.

The manual is what I was looking for. I bought the machine used and it didn't come with much and the learning curve has been very flat.

Thanks a lot.

[ger21]

Sorry, I also have a copy of Mastercam that I haven't even tried to figure out yet. Maybe it would work better?

The learning curve will be 10x steeper.

[WoodMizer]

Thanks, I'll be working on it all day today so I will hopefully get back to you soon with some good news.

Thanks for your help guys.

[crob09]

Just wondering how you set a 1/8" offset in Mach3, does any one have a couple of screenshots?
Thanks for your help and time.

[adprinter]

Wondering if any one out there can give me a hand.

I'm making a woodworking project and I'm trying to set up my machine so that I can drill pilot screw holes with a 1/8 tool and then switch the tool to a 3/8 compression bit to cut out the piece.

Just wondering how I do this in lazycam and/or Mach3. It looks like there are multiple ways to set it but so far it doesn't seem to be recognizing anything.

I would need to tell the machine what tool I want to use on a specific chain, to pause so I could change the tool in the spindle, and then restart with the new tool.

At the moment I think the machine is not recognizing the 1/8 tool diameter and is cutting a circle instead of a straight plunge for a 1/8 hole.

Any help would be greatly appreciated. I've looked at some of the tutorial videos on ArtSoft.com and it doesn't show much or I just can't find it.

Thanks,

WM.

I use Corel Draw to design all artwork for my machine. And LazyCAM to create the G code tool paths. LazyCAM works very well..... once you gain a correct comprehension of how to set things up. I routinely can drill holes, and cut profiles using the following method:
1- For hole locations (to be simply drilled) I create circles in Corel Draw with a diameter of 0.001" The actual diameter of the hole, is controlled by the actual tool diameter I am using to drill the hole. LazyCAM will still move the tool in a circle, but only a one thousandth of an inch diameter. Which Effectively simply drills a hole. Small diameter tooling probably has at least this much run-out TIR anyway.
2- For profile cuts, I simply draw the desired lines in Corel Draw.
3- I use the Export function in Corel Draw to export the file in the HPGL (PLT) format. This is very important, since the DXF export in Corel Draw leaves a LOT to be desired! The PLT export will preserve proper scaling of the drawing.
4- I then launch Mach3, then LazyCAM. Once LazyCAM is up and running, I use the File, Open Vector File option, and scroll down to select the HPGL (PLT) format option, and navigate to the folder where I exported the file from Corel Draw to select it.
5- The file is imported into LazyCAM. I then click on Option, Autoclean, to have LazyCAM automatically separate the various components of the drawing into separate layers. (Inside, Outside, etc.)
6- Once the various components have been assigned different Layers in LazyCAM, each Layer can then be assigned it's own tool, and cut depth.
7- The autoclean function in LazyCAM generally does a pretty good job of moving the various components (chains) of the drawing to the proper layer needed, but it is not perfect. You may still need to indiviually select chains (simply click on them in the Project tree of LazyCAM, and drag to the correct layer).
8- If you run out of layers, simply right-click on the desired chain to select it, and Send to New Layer. The cut order of the various layers will be performed from the top of the list (Project Tree) to the bottom. So, if you need to do things like drill a pilot hole, you will want this operation to happen prior to a profile cut (which cuts the outside lines, which would then leave the part removed from the work piece stock).
9- Play. When creating the tool table, you will want to set the "Depth of Cut per Pass" to a very shallow value (particularly with small diameter tooling) to AVOID a plunge full-depth into the material as this will often result in a broken bit. This will cause LazyCAM to create multiple passes to complete the particular chain. I.E. a 1/8" diameter hole cut to a depth of 1" (with the Depth per Pass set to 0.050") would "peck" drill the hole 50 thousandths deep at a time, until the cut depth of 1" is completed. In this example, it would take 20 passes (or "Pecks") to complete the cut depth.
10- If you have created your drawing at the actual size you want it to be cut out, then you will want to create an offset in LazyCAM, so that the actual tool path will cut the profile out to the proper size. You do this, by clicking on the profile chain (or chains) to select it (or them), and selecting the Offset tab in LazyCAM. Which will open a window prompting you for the Tool, and whether it is to be an Inside or Outside profile cut. Play around with the various options in LazyCAM......It is the best way to gain a comprehension of what is happening in LazyCAM, and the best way to learn how to control the machine. I like LazyCAM for this reason. It kind of forces you to learn the basics of what happens in a G code program. Even if you later move on to a more powerful CAM program, the basics you will have learned in LazyCAM will equip you to be able to "know" where things may have gone wrong when problems arise.
I have been doing this now for almost 4 years, and am still amazed at what can be accomplished. Mach3 does not care what tool is actually in the machine. It only reads the TOOL NUMBER. Make certain that the "Ignore Tool Change" option is unchecked in Mach3, so that any tool changes created by LazyCAM (or any OTHER CAM program) will be properly carried out. It is probably easiest, to create a "Hard Copy" list of tooling (A printout on a sheet of paper kept near your computer to refer to, when working with LazyCAM, or any other CAM software you may be using). The printout should include:
Tool Number, Tool name (for YOUR reference) I.E. 1/8" End Mill, etc. Tool diameter, Tool length (this depends on your machine, and the particular CAM software you may be using- but can be largely ignored if you don't have an Automatic Tool Changer on your machine, since you will want to Re-Zero the Z axis at every tool change- make certain to use the same reference point on your work piece stock when Re-Zeroing the Z axis after changing tools). The main thing to remember, is to get all your software "On the Same Page" (I.E. the printout of your tooling). So that when you create your tool paths in your CAM software, Mach3 will stop the machine, and wait for you to change to the proper tool before continuing with the cut cycle. Sorry for the "BOOK" response, but I remember how frustrating it was for me, when first starting out.