PW 2 problem

[phil_o]

I drew a heart by drawing a left half and then mirroring to create a symetrical heart. I grouped the two halves together. Then I created a cut file with a profile cut, and selected an outside cut. The half heart that I drew was cut on the outside of the vector and the mirrored half was cut on the inside of the vector. I tried drawing other symetrical objects with the same process and got the same results. This doesn't seem right. Am I doing something wrong or is there a glitch in Part Wizard?

[greg_russell]

Phil,

I have experienced the same problem when mirroring, and with using the transform tool to turn parts 180 degrees. The only solution I have found to this point is recognizing that I am going to have this problem, and make two separate tool paths. One cut on the outside, and one to cut on the inside. The one that is mirrored I set to the inside, knowing that it is actually going to cut on the outside.

It seems to me as well that there is some kind of glitch, but who knows?

Greg

[Brady Watson]

Phil,
You can't simply mirror the part, group it and run a toolpath on it, unless you want the results you are getting.

You have to close the vector by joining the two halves together. This involves 2 steps. 1st, select both vectors (provided that there are intersecting starting and ending points), then right click on them and choose Join. After you have joined them, they are really only joined in one place...you must then either right click and choose 'Close' or go to the toolbox and click on the close icon.

This was a big problem for me when I started using PW...now I know that it needs to be closed completely. If you have overlapping or open vecotrs when you group it, it will be blue in color. Pink vectors are completely closed.

-Brady

[gerald_d]

Brady, what you described here may be of interest to AutoCad users. To do the similar process in AutoCad, use the BOUNDARY command/icon - click anywhere inside the space formed by the heart halves and AutoCad draws an enclosing polyline right around the object. Joined and Closed all in one click. BOUNDARY is probably the neatest command in AutoCad for CNC work.

[Brady Watson]

Gerald,
That sounds like a really nice feature. I know that it would come in handy when doing intricate designs.

Phil & Greg,
I forgot to add that if there are not intersecting points on the 2 halves (there should be if mirrored...but if you have another design...) You can add points by selecting one vector and using ctrl + i, or the right-click context sensitive menu. Then select the other vector and insert another point in the same spot where you did the 1st one. Now you can join them. Be sure to zoom all the way in when adding points. Using the guide lines really helps with this because you can snap a point in an exact location. You can delete points by right-clicking and choosing delete point (or ctrl + d) and remove spans with ctrl + r.

You can verify that a vector is closed completely with no breaks by grouping it. If you see small circles when grouped, this is telling you that you have two or more points overlapping. You can delete these points and try grouping again. You also want to make sure that you don't have any loops that cross under like a pretzel. In this case, you can add and delete points and move points around until you get rid of the loop.

Learn to use the short-cuts in PartWIzard. They will greatly increase your efficiency and quality of files. 99% of the problems that I have encountered with my machine not cutting properly had to do with me not properly preparing the file. You can see in the pic below that there are upper-case letters on the menu beside each command when you right click on a vector. These are shortcut hot-keys that can be activated by holding down the control key and the letter.

Sorry so long-winded, but I think that this is of value for a lot of users.


4235


Hope that helps,
-Brady

[fleinbach]

I agree that joining the two halves as Brady explains is probably the best solution in this application but I found another way too be able to switch which side of the line will be the inside or outside. Last week I was cutting treated 2 X 10 boards with an arch on each end. I tried grouping them but had the same problem, one cut was on the inside of the first arch and the second one was on the outside. I disscovered that all I had to do was change the start point on one line to the opposite end and then when grouped the cut path was on the proper side of both arches.

[paco]

Or you can use de reverse vector(s) function too...

4236

4237
Note that I did'nt closed the vector for this example...

[Brady Watson]

Frank,
If you were just putting an arch on each side (as open vectors right?)...You could also use a Machine Along Vector toolpath and just offset it 1/2 the distance of the cutter diameter.

-Brady

PS- Are you making it up to Bill's Camp?

[fleinbach]

Yes, Brady you are right, I also thought of another method that would have worked but for some reason the one I choose was the one I described above.. As always there are several ways to skin a cat.

Yes, I intend on being there. Actualy I am supposed to be at the program session on Friday also but it will depend on whether I need to be on a job site that day. But I am 99% sure I will make Saturday.

[greg_russell]

Brady,

Thanks for the pointers. When you say offset using the machine along vectors tool, are you doing this with the "tolerence" variable? If so, does this mean that a positive number offsets to the outside, and a negative number offets toward the inside?

Greg

[Brady Watson]

No Greg...I typically NEVER touch the tolerance setting because I know that I will forget that I changed it...and consequently be scratching my head wondering why something was off spec. LOL!

I always offset the vectors using the offset tool (or do this in CAD and import both vectors). For instance, If you were using a .25" bit and chose Machine Along Vectors, then you would offset the original vectors 1/2 of the bit diameter, in this case, .125". That way, the edge of the tool will ride on the inside or outside (whichever side you chose to offset) of the vector. Think of the Machine Along Vectors strategy as centerline cutting...the center of the bit rides along the center of the vector.

No, it doesn't always work out that a positive/negative number will offset to a given side in PW. It is more dependent on where the start point of the vector is (I think...)

Does that make sense?

-Brady

[dingenis]

greg,

toolpathing a open line in PW2
OUTSIDE toolpath- places the toolpath on the righthand side of the line, seen from the start point.
INSIDE TOOLPATH-places the toolpath on the lefthand side of the line, seen from the startpoint
it does so also when the toolpaths are grouped
i use the Allowance setting to offset toolpaths

hope this helps
dingenis