Some Frustration Points of using Aspire, Shopbot Desktop and a Wide Z Project

[Chazz]

Hi folks,

I am still working on the guitar neck and have had what I would call Brute Force success. It seems like some of the things that I am doing in a round-about way would have some better way to deal with. Some of the things, I just have not found a way at all...

1) One of my biggest problems is when I am trying to do the 3D cuts on materials that have a rapid changing Z slope, there doesn't seem to be anything to account for the chuck or that the bit only has 1" exposed. It seems to want to plunge to the spoiler board if it is on the edge. So far, I have managed to just limit the toolpath area so it can't get down there (for the rough pass at least). However, my initial rough pass was with a 3/4" bit and it worked great clearing the bulk stuff away in record time. Of course, not much definition. So, I would like to make a second "rough" pass with a 1/4 bit. As my material started at 2.8" tall, it wants to start milling from that height. I can find no way to tell it to start cutting from 1.5" rather than the 2.8" of the project. Yes, I can change it, calculate, change it again; but I wish I knew how to make it just make use of the headstart of the 3/4" toolpath. Optimally, I could tell it to use the 3/4 rough pass as the starting point and continue from there.

2) I had to do lot of the rough running with manual surface planing to remove material so that I would know the chuck would not hit it. My waste material that I had glued to the sides to hold it down was high enough that the chuck would hit it as it was working just a regular rough pattern. I needed it that high for then I milled the other side which I did first. Once flipped, the purpose of them being that high was fulfilled. But they were now in the way. So, I milled them down with surface planing plans.

Well, there are other points; but this is enough for now.

[Brady Watson]

Chazz,
Without chaos and confusion, there can be no real learning going on. What you describe is par for the course when it comes to machining non-decorative three dimensional parts. Not to worry...once you get some success, the steps and parameters you'll need to operate in will become 2nd nature.

The DT in stock trim, even with the extended Z, is a poor hardware choice for machining necks. You can squeak by on electric, but acoustic necks, forget it. Now you've already made the investment in the machine, so you might want to consider modifying it to better suit your needs. I think there is a post here showing a very long Z axis that Max Girouard made for his machine - I believe for machining necks to get that additional Z stroke. This will allow you to use longer tools and in turn, jump through less hoops to do your work.

Pursuant to problem #1, a longer bit and Z axis will solve the collet collision issue. In terms of Aspire and eliminating tool 'fall off', I'd suggest making 2 vector boundaries; one for your roughing pass and another for your finishing pass. The boundary for the 3/4" roughing tool (I would use 1/2" BTW), has to be larger so that the bit can fully cover the whole area. For 3D finishing, try using the fit vector to relief tool and then offset that 1/2 of the finishing tool diameter. Run a 3D finishing preview in Aspire and see how deep it goes. If it falls off, offset it inward a little, or use node editing to move it in enough to prevent fall off. This is normal - it's not just you.

By far the easiest way to get a toolpath to pick up at a specific Z depth without reinventing the wheel or redoing the file is to just calculate the toolpath as-is and save it out as an SBP. Open up that SBP and scroll down to where the Z gets to be where you want. Then delete all of the air cutting lines (where Z depth is less than where you want to start, all the way up to the very top - with one caveat. Make absolutely sure to keep everything above the very first M3 command at the top of the file. Make sure the tool can safely get over to where it needs to go at safe Z height. This may mean copying and pasting the first M3 move at the deeper Z depth (where you scrolled down to) and then replacing the M3 with a J3 and the last column (the Z height) with your positive safe Z height so that it traverses over everything with no collisions. Once you do this once, you'll then know how to do it going forward. It's not hard.

For #2, I'll just explain how I have machined these 2-sided parts and you can see if it makes sense to you. First, I always prep my material in XYZ by planing or mic'ing the dimensions precisely. It is very important for 2-sided milling, especially the Z and whatever axis you flip in. I usually flip in the Y direction with the X axis being the 'axle'. I have the X & Y edges of the MDF spoilboard on my machine precisely aligned to X & Y, using the spindle with a bit dragging on the edge of the loose board to align it. I keep going until it is perfectly aligned. This gives me a perfect edge to reference my material for 2-sided machining. If your board is not square, an end mill can be used to square it up to the machine's axes.

I hold these down with carpet tape & align to the front & left edge for XY alignment. I first run a profile pass with tabs around the entire perimeter. This provides some relief for the finishing tool and gets rid of any cusps down where the fingerboard mounts. Then rough it with a 1/2" 2-flute end mill. Then finish with a 1/4" ball. Then we do the flip. Clean it off and re-stick it to the bed using the front and left edges again to align it. If your board isn't square/parallel, then you are going to get a step from one side to the other...material prep is key. Repeat the roughing and finishing on side 2. If you are worried about not having enough meat for side 2, make the tabs long and thick. You can even make them full material thickness and trim them by hand.

-B

[gc3]

work around is to learn how to "trick" software

100mm blank...82mm doc...

76.2mm blank...63.5mm doc...

[Chazz]

I am working the guitar for someone else who is doing the actual building of it. So far, LOTS of learning has taken place.

I do have the extended Z kit for the DT; but didn't want to put it on until after this job for fear of breaking it completely and not being able to proceed. I have managed to make it work with just 4" Z... it is a story worth documenting as I plan to do on the second one that we are planning.

My latest frustration is that, when in 3D rough cutting mode, for a given area if there is no model, it seems to gravitate to a specific Z height for the lowest cut. I can't see how to change it at this time. I will go back and revisit the various controls to figure it out. In my case, this Z is HIGHER than my model area and leaves enough material to give me worry.... requiring my 1/8 bit to cut upto about 1" of depth at one time!

I had not considered editing the sbp file by hand.... I will have to look into that. Once I have, is there any way to "preview" it in Aspire? I am more use to VCarve v7 and just learning the Aspire stuff...

253522535425353

The first is the model, the second is rough pass using a vector boundary and zero offset, the last is the same with 1/2" offset. The extra area is higher than the area over the model.... I will look at the model setup options....

[adrianm]

You can use the previewer built into the SB software to preview an edited SBP file. It's made by Vectric (who make Aspire) so it should be pretty familiar to use.