Anyone who has done this have any advise? I am going to add pins to my machine so that I can consistently register fixtures that I make and general work. I know you have to make sure you set safe height I am talking about the drawing and actually adding the pins then using them with some type of offset. I am using the latest version of Vectric Aspire. I have an AR8 Pro.
I know there is a way to change what home means not sure if that is temp or permanent and I suppose you could always create a tiny bit of GCode to replace the "macro" in this video and run it.
This YouTube video is my starting point.
Last Edit: Feb 5, 2022 13:56:27 GMT -5 by gene35146
Not sure if this helps, but on the RichAuto controller the origin may be reset to the current position of the spindle with the "XY --> 0" button. It is not permanent. The tricky part is accurately and consistently locating the position of your origin for that job if it is reset due to machining a different job. You can always use absolute coordinates to find the best location, which may require some trial and error, and then record them so that you can go back to that absolute location and once again press the "XY --> 0".
I'm doing 2-sided machining, so my technique for solving that registration challenge is a bit different than yours, so unfortunately I can't add anything further that might help out.
I am actually in the process of doing this myself. I am swapping out my MDF slabs that came stock on my AR6 with 3/4" 6061 aluminum bars. Once I get them installed and surfaced i am going to engrave around a 25mm x 25mm engraving on the table to easily see where I am putting in my material. I am also going to be keeping a master CAD file template that has my exact spoil board and locations of threaded holes as well as precision dowels like the video shows so after I design my part I can import it into the master file and I literally never have to change the x and y coordinates. Just Z (sometimes, more on that later). I leave X and Y zero at the home position and just use an offset when creating the job setups in Fusion 360. I also barely EVER use z zero as the top of my material as I do a lot of parts that have to have holes drilled all the way through. Here is an example of the job setup (the full idea is not in the photo as I am still finalizing the design of my new spoil board setup):
If you can see by the photo the material is exactly 100mm on the y axis and 25mm on the x axis. Since I have an engraved spoil board like this:
This allows me to place the material comfortably and use clamps without any guess work regarding collisions. And if I use the Z zero as the top of the spoil board I never have to worry about a plastic cutting endmill getting destroyed by my new aluminum spoil boards later on. Plus this prevents me from needing to take a caliper to each piece of material which saves time. Once I get the dowel pins working I can definitely post a video about it.
You have 9 different locations that you can set and recall at any time/ Press the Menu button and a number (1-9) when you have your location.
Home your machine, then move to a location you want to store for your jig, then press the Menu button and a number to store that location.
how do you store those locations? I know that when you stop in the middle of a job you can save the break point. But how do you do that without running anything, just after moving the spindle to the origin?
To store those locations, use press the Menu button and one of the numbers (1 through 9) at the same time, move to your desired X0Y0 location, and zero out XY. That location is now the origin for that particular work zone. To return to that particular X0Y0, select Menu + <work area number you want to use> and then hit Origin. It will return to wherever you set your XY0 for.
By way of example, I have a rotary axis, so I created a work zone for that attachment (I use #9, just so I don't accidentally over-write it), and created an origin in line with the center of the attachment (X axis), and about 5 inches away from the rotary axis headstock. Since I normally leave my rotary attachment mounted, I just have to select Menu+9, and hit origin, and it moves to that precise location, every time. The biggest thing to remember is NOT to zero out your XY axes when it isn't in that location (VERY easy to do by accident). It also helps to mark down your zone Origin, relative to the machines home position, in case you do accidentally zero out the XY0 by accident, and mark it in pencil (or on tape, etc) near that work area (for example, for my rotary attachment, it might be X23.6 Y421.3 (in mm)). If you do mess up, go to home position, and then using your controller you can enter the coordinates into the controller (I forget the exact process off the top of my head) or move there manually by jogging the controller.
I really like this feature (work zones) and I use it when I am doing multiples of the same item on a piece of wood (let's say I'm making 3 of the same item, BUT I don't want to do them all in the same project sheet (in Aspire). I can set up one work zone at the bottom of the piece of wood, set up work area #1; move up to the area where the next piece will be cut out, and set up work area #2, etc. You can keep the same bit in the machine, and select the new work area (ensure Z0 is correct for this new work area) and then select "Repeat Machining", and it will repeat the previous toolpath. You COULD program a toolpath in Aspire to do 3 at a time (using my example), but if the wood isn't perfectly flat or straight, you'd have to program those variations into Aspire, and if you need to repeat a particular toolpath, it would have to re-do ALL of the pieces, just to fix one area for example.
This might be confusing, but it really is a good way to do multiple pieces, even on completely different wood types, set up anywhere on your work surface. NOTE: I use the center of my workpiece/model for X0Y0, always. I have also started using the machine bed for Z0 (after 6 or so years of using a CNC router....), which makes way more sense than using the top of the material surface. The Z0 can be set ANYWHERE you want; it doesn't have to be set where the X0Y0 (which is the way I used to do it, starting out, and it became a habit). It's ok for 2D work, but if you're doing 3D crests (for example) you can end up milling away the area you set your Z0 height, and then you are screwed: where do you set off Z0 height for follow on toolpaths?
Thanks Allan, very informative. Will try that. So, you move it to the work area, save it, and then go to the X0Y0 for that work area, zero it out, and the next time, when I turn on my machine after a week or so, I just hit menu+work area number, and hit origin and it move to that zero position (coordinates showing zero), right? That is cool...
Yes, I also tried once to Z0 on the spoiler bed...actually, it keeps your spoiler bed almost intact. BUT, when the material surface is not even I am worried to cutting too much away...but I agree, it is the better option, I should get used to it.