ShopSabre and Optiscout

[Signed Out]

We got a ShopSabre Pro510 this past month and getting up to speed with it. It has a 10 hp ATC spindle, tangential knife and optiscout camera.

I'm planning on cutting a lot of aluminum and dibond signs through optiscout and tons of holes. Some of the settings in optiscout are either limited or I'm not understanding it correctly. I'm able to get the system to read registration marks and cut correctly for the outside shape of the signs. Took me a few tries to figure out how to do multiple passes here or onion skin it, but having more trouble with the holes.

First I tried a .1875" o flute upcut bit with optiscout set to cut inside diameter of a .25" circle for the holes, for some reason I got .375" dia. holes, so I guess inside means to center of tool?? Then I figured out how to replace the circles with "drill marks" so they are basically single nodes that look like a target. But here I'm still only able to drill straight down, no spiral cut options or peck drilling that I can find. So I drill straight down with the same type of bit but .25" and it cuts the holes fine, but it's pushing the chips through and between my sheet and spoilboad and causing issues.

So I'd like to try a regular drill bit for the holes but having trouble figuring out how to drill a little into the spoilboard so the tip of the drill bit clears and the full diameter of the cutting edge makes the holes. Optiscout uses the low boundry as z0 and you can set it wherever you want really so I know how to get it to go down further than the top of the spoilboard. But is there a way to be able to have some tools go that far and others not? Do I just need to wrap my head around the depth sttings in optiscout and "trick" it somehow? Or can I maybe adjust the tool height for just the drill bit I want to go deeper?

Any thought any optiscout/shopsabre users out here?

 

[JBurton]

Oh glory, someone else trying to learn optiscout on a shopsabre!
It's a nightmare compared to colex and stuff, but it can work. There should be settings for inside/outside cuts, I'll have to fire it up and take a look, but for drilling straight into the table top, you could easily do this by loading a bit, measuring the tool via tool height, then unchuck the bit, and pull it out another 1/8" or so. This will cause other issues, like plunging and tool approach needing to be adjusted to keep it from hitting the material at full speed, and you'll want to be wary of dragging the bit across the table top/material.

 

[Signed Out]

Oh glory, someone else trying to learn optiscout on a shopsabre!
It's a nightmare compared to colex and stuff, but it can work. There should be settings for inside/outside cuts, I'll have to fire it up and take a look, but for drilling straight into the table top, you could easily do this by loading a bit, measuring the tool via tool height, then unchuck the bit, and pull it out another 1/8" or so. This will cause other issues, like plunging and tool approach needing to be adjusted to keep it from hitting the material at full speed, and you'll want to be wary of dragging the bit across the table top/material.

About half of what I've learned about optiscout has come from your posts, so thank you!

As for re-chucking the bit, I thought I read or saw on a video somewhere that you can change the tool heights in the shopsabre controller after doing an auto tool height. I think that might be the way but I'm not sure how to do it.

I tried the setting in optiscout for inside cut, but it seemed to use the center point of the bit rather than the outside diameter of the tool to cut the inside of my holes.. I'll have to give that another go.

ShopSabre has been good on the support end, but they just don't seem to know all the ins and outs of optiscout. It seems like there is a ton of functionality in there that could be utilized.

 

[JBurton]

you can change the tool heights in the shopsabre controller after doing an auto tool height. I think that might be the way but I'm not sure how to do it.

I'd avoid doing this in settings really, unless you plan to do a lot of the same hole drilling...
Simplest thing if it's only occasional, would be to stick the bit out 2", and then use a second tool holder that is sticking out 2 1/4", measure the short tool, then swap the tools manually when you want to drill into the table top.

Actually, simplest would be to get an endmill router bit working properly in optiscout. Are you exporting the inside and outside shapes on the same layer? It should treat the holes as insides and the outer edge of the shape as outside without much effort.(I'll have to verify this on screen, but I believe if you zoom in on the edges after assigning layer options, the 'part' edge is a dashed line, the 'cut' line is solid.)

I'll shoot a picture of my settings that I use to make a .125" bit work, hopefully it helps clarify what settings you will want to set it up to.

 

[JBurton]

Here are the settings that properly cut on the outside of my shapes, using a .125" bit.

 

[Signed Out]

I did what you suggested and just pulled the drill bit out after getting the tool height, worked out good.

I see you have your "final pass depth" set at .125". I was under the impression that should be set to 0 if you want it to cut all the way through to the z low boundry/top of spoilboard?

I've also found some videos from jwei jcut showing optiscout with what seems like a lot more options. And then I looked through the optisocut help section and it refers to a lot of stuff that doesn't seem available on my computer. Check out this video

on youtube at about 3:40 shows "router multipass" mode output parameters.. I'm wondering if we can access these same modes somehow?

 

[Signed Out]

Here are the settings that properly cut on the outside of my shapes, using a .125" bit.
View attachment 177140

 

[JBurton]

I see you have your "final pass depth" set at .125". I was under the impression that should be set to 0 if you want it to cut all the way through to the z low boundry/top of spoilboard?

I don't think so, but to be honest I'm not using the software frequently enough to say that this setup will work as intended. Here is an exchange I had with shopsabre while trying to reckon all the meanings for these numbers:
My email:

Ok, so I often reference my table top, but I am referring to the top of my spoilboard, as I have covered the entire table with mdf.
When initiating optiscout, I put the bit on the top of the spoilboard, punch g37cal, and it goes to measure the tool. At this point, I have a panel ready to get cut, with it's top surface at Z+.125. Here is where it begins behaving wonky.
When I go into Opti, and set the bit up with 0 depth, the scanning completes successfully, grabs the bit, then plunges to Z+1" (the material offset setting height), and it will execute just fine.
When I do it with actual depth input, it plunges to the spoilboard, then heads for the first panel, does a z up to the Z+1" material offset value, then plunges again and starts cutting, it will do this every time it has a rapid move to the next Z down move. Obviously the problem is the bit would cut anything on the table between the tool holder and the first cut, and between every other cut start point.

Screenshots for reference:

Shopsabre's response:

After talking with them I think the problem is your final pass depth. These guys are a German company, so their wording probably makes sense in German and in English their thought process is weird.



So Material thickness is what it says. Pass Depth is actually maximum cut depth, which they’ve done as a positive number down from the top of the material even though the zero is at the bottom. Depth per pass is what it says and then final pass depth needs to be 0 – so basically that’s the lowest it is allowed to go and will override the other settings. I don’t know why it’s like that. But basically:



the first two should both be material thickness, pretty much always.



Third, depth per pass, needs to be thickness per pass. So on a 0.125” material, a single pass would be 0.125, two passes would be 0.0625, etc



Fourth, final depth, should be 0 because we want it going all the way down through the material to 0.