Wrong size circles

[sbd1]

I'm still getting acquainted with my setup, so I'm hoping this rather embarrassingly simple question will be easily answered.

I'm trying to cut a circle 2-3/8" in diameter, but I keep getting 2-1/4" circles instead (it's only being cut 1/4" deep).

I created the vector (2.375" diameter) & toolpath with AC2008 then saved the SBP file using 'Arc Inches'. The toolpath settings are:
2D profiling
Profile side: Inside
Final pass thickness: 0.1
Final pass allowance: 0.05
Profiling tool: 1/2" straight
Cut direction: Climb
Lead In/Out Moves: Distance 0.2, Overcut 0.2, Circular arc Radius 0.25

I haven't tried cutting these circles with SB3. All of the straight toolpaths I have created recently in AC have been accurate. Can anyone see anything wrong with this?

[steve_g]

I think you need to cut out side the profile

Steve

[steve_g]

oops... I was assuming you want the disks and not the holes...

Steve

[garyb]

Its because you are using a final pass but only running the one toolpath.
When using a final pass allowance it creates 2 toolpaths, you need to save them in the correct order and to the same file the final pass will cut to the correct size.
Gary

[sbd1]

I think you have it correct Gary. I now see the 2 toolpaths in AC & don't think they were both converted into the SBP file I created yesterday. I'm heading over to the shop now & will give your 'two-in-one' SBP file a try on the machine. Thank you!

PS. Any idea why I keep getting the attached error message whenever I create the SBP file from this toolpath?

PPS. Is there a way in AC to have it not pull the Z up to safe height between repeated plunges in the same hole?

[garyb]

re the error: it's hard to say without knowing what steps you took, just delete the lead in's recalculate then add them back in. You may have got out of wack doing an edit.
don't forget the lead ins will be added to final pass toolpath as well.

Is there a way in AC to have it not pull the Z up to safe height between repeated plunges in the same hole?

which toolpath strategy are you referring to?
Gary

[sbd1]

Gary, it appears there was a problem with one of the six circle vectors I had in this file because I got another error message & then that circle turned red. So I deleted it, redrew it & now I don't get the Toolpath Manager error. Not sure what happened to that circle because they were all drawn exactly the same way but I'm glad to no longer be getting error messages.

When I asked about the Z pullout & return I'm referring to the 2D profiling toolpath I'm using to create these circles (holes). I'm using a 1/2" bit setup with 0.5" stepdown & my final depth set to 1.55 with a final pass thickness of 0.1. Doesn't that mean the Z should plunge down 4 times? What's actually happening on the machine is:
1) After each of the first 3 plunges the Z is pulled back up to 1" above the table before returning to plunge again (or moving to the next hole on the table after the 3rd plunge).
2) The 4th (final pass) plunge is not completed until after all the holes on the table have been plunged 3 times. I can understand this if I wanted to use another bit, but I don't. Is there a way to complete all 4 plunges (3 first pass & 1 last pass) in the same pass while the router is each hole?

BTW: Thank you for your catch regarding me missing the final pass toolpath in the SBP file. The circles are now cutting very close to the size I asked AC to create. They are cutting -0.025". Does anyone know if this is considered normal for these machines?

[garyb]

Darren
The reason it lifts is because the LP is a separate toolpath. because you have selected all your circles, it will do all the 2d profiles first then come back and do the LP.
Don't know how many circles you have but you can toolpath just one circle then copy/block copy the toolpath then merge and that will do what you want.

the other option is to toolpath ea circle separately then merge them in the toolpath list selecting the options to merge in order as list and to preserve, this will also do what you need.
Gary

[MogulTx]

Daren,

I have noticed that the program may recognize thickness of the line drawn and cut to some specific point --maybe the outermost edge of the line, maybe it is the center of the line, maybe the inside lip of the line. I kept getting confusing results until I went into my design program and selected a line width of .000 and a scale factor of 1.... then output a dxf file to use in Aspire (actually discovered this trouble in Part Works a while back, before I got Aspire) .... Once I started doing this, the machine has been very reliable on dimensional output.

I also use a caliper on my bits to ensure they are appropriately sized to the expectation. I have had some that were "off" by a bit. It makes a slight difference, but should not make an .02" diff, unless you really have a mis-marked bit.
MGM

[sbd1]

Gary: Thanks for the info, it's definitely appreciated! When I toolpathed one circle then copied it, I am able to produce a SBP file that shows both the 2D & Final Pass cuts being completed on the 1st circle before moving to the 2nd. However, the bit is still being pulled up to 1" between plunges (bit stepdown is set to 0.5" & finish depth is set to 1.55"). Is there any way to have AC just plunge deeper after completing the previous partial-depth plunges? Or is this happening because I'm asking it to do lead in moves?

MGM: I'll watch for that when I next import lines from another program. For these circles, I created the vectors in AC. After reading your comments I even checked to see if I could see/adjust the vector's thickness, but I can't find that info anywhere. PS. I also checked the bit size & it's accurate. I've recently just adjusted & tuned the whole machine so there should be minimal play in all axes, so at this point I'm not sure what could be causing the size discrepancy.