only half the design cutting when tiling

[Hoytbasses]

Greetings:

o.k..... we're trying to cut some fender style guitar necks on the desktop.

we created the design and toolpaths... and set it up to tile on a vertical plane.

when we cut the piece, it aligned perfectly, looks great BUT only cut the left side of the design!

see attachment (if it will take a PDF).......when I look at the tool paths they are highlighted as if they're going to cut correctly but it doesn't cut the right side of the part......weird!

thanks so much for your always helpful responses....

Karl

[Hoytbasses]

I think I might have figured it out:

when I was in shopbot 3 and previewed the toolpaths, it doesn't recognize that I had used an offet of 1.5 (x) when setting it up. It shows the material in preview mode as lined up with 0,0 instead of 1.5,0 which is where the material is located......

so how do I get the tiling toolpath to recognize the material is offset to 1.5?... or do I just set the material up to reference at 0,0?

thanks in advance

kfh

[steve_g]

I think TJ needs to do a class on “offsets”… My use of them has been unpredictable at best!
SG

[scottp55]

Steve, I second the motion. First time I tried a Z offset almost hit my extrusion table-Thank You Spacebar!

[Brady Watson]

... or do I just set the material up to reference at 0,0?

We are talking about origin offsets in Aspire/VCP right? If so, yes. If you physical part is sitting at 1,1 in relation to your physical spoilboard, then you setup that location in Aspire/VCP as an origin offset - which will now be your 0,0 location. The usual 0,0 location at the bottom of the screen will now be -1,-1. Hovering your mouse over that area in CAD will show you where you really are. When you setup, your origin offset will most likely be a negative number in the Vectric stuff. (You'd enter -1,-1 for a 1,1 offset)

I've only used offsets in SB3 a handful of times because I like to see what I am going to get in CAD/CAM. I just set the offsets up in Aspire. This minimizes confusion.

Some may ask, why use offsets at all? One example would be if you are machining some 3D stuff and your boundary vector or toolpath goes off of the model space, causing the Z to lift off of the relief. By moving the origin up, you get full access around the model, but you still need to make sure your model space is large enough to contain the entire operation.

Make sense?

-B

[Joe Porter]

I'm thoroughly confused. It looks like you need to feed through in the X axis, not the Y, (looking at your piece on the table). As far as off-sets are concerned, I have never used them or seen the need to, but that's just me.. I am talking about the Vectric program. There must be a reason for them, but I don't know what it is...
When you saved your tool path, did you have the checkbox checked for saving a Tiled tool path? You should wind up with two tool paths, T1 and T2. You run one, pause, move your material, and then run the other. I hope this helps...joe

[Brady Watson]

Karl,
I think I understand your question now...Read the help file in Aspire regarding toolpath tiles. (search "Toolpath Tile") - it explains about overlap and how that can make the tool over cut in order to prevent uncut or 'cutter cusps' at the transition of the two toolpaths.

You will want to make sure that if you told it you wanted 1/2 the cutter width (say you use a .25" ball - so .125" overlap), you would setup your part as if you didn't have any overlap...and the tool would machine AN EXTRA .125" in the Y at end of the first piece. You just want to make sure your tool has enough room to 'over travel' and not hit the hard stops. So with a 16" tile, you would go a max of 16.125" in the Y on the first toolpath tile. Make sure your tool can. (It should go at least 18")

So...in terms of 'offsets' - no. There is no need to apply an offset. First piece gets set at physical Y0 & run. Material slides back exactly 16" in -Y and the 2nd tile is run. It is easy to over-think tiling, especially when there is an overlap. Sorry for the confusion - 'offset' can mean all sorts of things...

Joe - He can't tile in the X. It is a Desktop. It would interfere with the gantry.

-B

[Brady Watson]

I forgot to add that you can verify what your machine will do by just opening up each SBP and take a look at the code. Pay attention to the Y values at the beginning & end of each file (assuming raster toolpath) to get an idea where it will go. It is a good way to verify what is really going to happen at the tool if you are unsure.

-B

[Joe Porter]

I didn't realize that the Desktop had a different XY arrangement from the Buddy. I really would be confused! Just when you start to think you have things figured out...Oh well....joe

[Hoytbasses]

Thanks for getting back to me:

I'm working in Vcarve pro.

and Joe, it has the same XY arrangement, I think I misspoke. I had a fence on the table on the vertical axis that was lined up with x=1.5"

we tend to use the offset feature a lot. the main reason being that it's great to have a hard fence for kids (remember, I'm working with high school kids) to reference stuff like signs, smaller parts etc. I went so far as to install threaded inserts into the table so I can easily put on/remove the fences as needed. In this case, as it's a desktop, I used the 1.5 fence on the Y axis so that the neck blank could rest against it. The actual tiling procedure went exceptionally well, but only half of the neck was cut out.....

Then.... I went back and re-read the Tiling section in the help files......(when all else fails, read the manual )

it clearly states that the tiling feature references at 0,0! so when I loaded the part into the machine with an offset of x=1.5, Shopbot 3 didn't recognize it hence the cut file cutting 1.5" over from where it should have.

so today I'm going to run the same file using 0,0 as the reference point. I'm going to bet myself a Guinness that it works fine. If it doesn't I'll buy myself a Guinness as a consolation (win, win)

thanks so much, folks. I always appreciate the candid and helpful responses. I'm still a total rookie, but slowly figuring things out as we move forward.

Karl