Newbie software surprises and questions

[Ross Leidy]

Even mistakes with my new SB Desktop are not distressing because I can see that I'm going to have a grand time with my new machine. With the salve of a new acquisition, I can instead refer to mistakes as surprises. Here are a few.

* I made the assumption that when calculating toolpaths in Partworks that lead-ins would have been optimized to avoid cutting into adjacent profile cuts. This doesn't seem to be the case. All my toolpaths were calculated together, but I found that I ended up with a little divot that was cut into one of the profiles by a lead-in for another. Is this something I need to watch for manually in the 3D tab simulation?

* Is there a prescribed way to cut a right-angle x/y guide that's been mounted to the spoil board? I'm thinking I must have done it the hard way. I created a new PW design with an "L" for x/y guides, a circle over the vertex, welded the vectors, and then trimmed the hypotenuse that was added by the weld (can I prevent that?). I mounted an appropriately sized piece of ply into the corner of the spoil board, and in SB3, I ran TS to set the C2 offset to 2,2, and then cut the guides. It turned out fine, but it seemed like a lot of steps for what is probably a very common thing to do. Is there a better way to do this?

* While cutting through the guide material, I found that my cut depth was too shallow. I had Z-zeroed and mic-ed the material, but still it was too shallow. I had to go adjust the thickness 2 times in Partworks, recalc the toolpaths, and re-run the sbp file twice to finally cut through. Is there a way to run the job but offset Z just a bit to achieve the same result? I looked at the dialog that opens with FP, but it wasn't clear to me that I could alter any of those settings to make that happen.

Thanks for any advice,
Ross

[steve_g]

Ross

As I understand your questions...
Lead-ins are usually carefully calculated to avoid nicking other parts... it's not unusual to get a message that a lead-in has been modified or eliminated to avoid conflict. Is it possible that the divot is caused by dwell at the end of a path without a lead-out?

If I understand your question... you should use the fillet tool with the dogbone option to create the inside corner clearance you're trying to achieve...

I would re-zero slightly lower and run the same tool path again... is it possible your Z-zero plate thickness is wrong?

Hope I've answered your questions... if not ask again!

SG

[myxpykalix]

Is this something I need to watch for manually in the 3D tab simulation?

you have to space your parts out far enough apart to allow for the diameter of your bit plus some material to keep the blank together.

I created a new PW design with an "L" for x/y guides, a circle over the vertex, welded the vectors, and then trimmed the hypotenuse that was added by the weld
Whaaaat? I think i understand what you said...did you just say you made a 90 degree corner for material?:confused:

I found that my cut depth was too shallow.
Do you mean that you, for example are cutting 3/4 plywood, you set your depth of cut to .75 only to find that you have not cut thru your material?

When this happens to me, what i do is i just guess how much more i need to cut to go thru the material by going back to x,y 0,

then lowering my bit by doing MZ0 lowering the bit to the material surface 0
(while router NOT running)

then clicking the Z down maybe .10 and RE Z'ing to that lower height
then rerun the file, it will cut down .10 deeper on the ending but if you have tabs you need to be careful.

The idea is all you are having to do is re Z, rerun file

[adrianm]

Steve's answers sound spot on to me.

Just to add a bit more info to the guide question. The way I would do that is to draw two overlapping rectangles to create the L and use the Weld tool to make them one L vector.

Now you've got the inside corner of the L that will be rounded so you need to use the Fillet tool. Set it to the radius of the bit you're using and select dog bone and then click on the inner corner. That will create the correct relief cut automatically.

It's well worth spending as much time as you can spare going through the tutorial videos for PartWorks/VCarve (same program) at http://support.vectric.com

[bob_reda]

The "L" shape got me. I'm thinking you use this to line up your material. If you do you don't need a program. You want the material to line up with your machine. The way I do it is to lower a v bit or .25 em into the spoil board and with the key pad run a line both horizontal bring it to the side you want vertical and run it that way for a foot or so. Now you have two lines that are parrell to you x and y axis.

Bob

[steve_g]

For locating "one-offs" Bobs method works fine... If you have 100's to locate something like the photo works better!

SG

[Ross Leidy]

Thanks for the responses, guys. I think a couple photos would be in order here. The first shows the nick I got in one profile. The lead-in from the profile for the oval shape is what did it. There was clearly plenty of room between the two parts to avoid the nick.

The other photo shows the guide that I cut from a pieces of birch ply. I mounted the square piece of ply to the spoil board, ran through TS to set a -2,-2 offset for C3, ran the C3, and then cut the 90-deg guide with my part file. It sounds like I could have simplfied the proces by using the fillet tool to create the relief in the vertex.

Jack - thanks for the idea for resetting z-zero without the plate. That will be just the ticket the next time.

BTW, I used a variant of Brady's vacuum film technique in the first photo. For my table tennis paddles, I wanted to use a compression bit for crisp edges, so I need to cut in one pass with no tabs. Instead of coroplast, I used a scrap of corrogated cardboard box. Instead of vacuum, I used bands of double-stick tape between blank and cardboard and between cardboard and spoil board. I cut many different shapes of paddles, so I wanted to avoid cutting into the spoil board if possible. This technique worked great.

[Brian Moran]

Hi Ross,

Could you send the PartWorks file (crv) to support@vectric.com so we can take a look at it?

Thanks

Brian

[Ross Leidy]

Hi Ross,

Could you send the PartWorks file (crv) to support@vectric.com so we can take a look at it?

Thanks

Brian

Sure thing. I can send it out this evening. Thanks.

[Joe Porter]

Ross, instead of a "Lead In" I use the "Spiral" option. This starts at the top of the material and follows a spiral path to the depth of your cut. This gives a nice clean cut and eliminates any extra gouges. joe

[ssflyer]

As far as the right angle guide, everyone may be overthinking it a bit. I just draw a 90 degree angle with the polyline tool - the software shows when they are at 90 degrees. Then the dogbone fillet and an Inside/Left profile on it.

Cutting too shallow - you said you mic'ed the material, but have you ever Mic'ed your ZZero plate? Mine was off from the default, 0.121", so had set the actual thickness in the SB3 software. You should not have to keep going deeper to get to where you told it initially. I regularly leave 0.002" skin on the bottom of my material for cutout passes, to avoid using tabs or cutting into my spoilboard. (When doing this, I ZZero to the table)

[mark_m]

Hello Ross,

Thank you for sending in the file that you are having problems with into support.
As Jack mentioned above, you would need to take into consideration the diameter of the tool bit when spacing the vectors.
When machining the start of the lead-in with the diameter bit that you are using this will lead to the
"Paddle" being slightly nicked, this can be clearly seen in both the 3D toolpath
preview and the 2D preview when using the "Solid" option.
To avoid this, you would need to either re-space the two vectors, use a shorter lead-in, or alternatively, you could set a different start point for the lead-in.
If you were to insert an additional node point somewhere down the top left hand side of the oval shape, make the start node point and the lead-in will start at this point.

To do this, first enter node-editing mode (press N on the keyboard), place the mouse cursor over the oval vector at the place where you
would like the lead-in to begin cutting the vector. Type P on the keyboard. A new node will be inserted in the vector at this point and will become the
start point. Type N to exit node editing mode. Recalculate the toolpath, the lead in will now start a different location away from your
“paddle” vector and the toolpaths associated with that vector.

I have sent some picture of this in response to your email to support.

I hope that this helps.

Cheers,

Mark.

[Ross Leidy]

Hi Mark - thanks for the the details. I'm fairly certain that I had the correct tool selected - it was a 1/4" compression bit. If the bit had a larger diameter than what I specified, I would have expected the profile to come out slightly smaller than designed, but it was dead-on.

Assuming that the bit was specified correctly, should I assume that the software will calculate the lead-ins correctly? (avoiding nicking adjacent profiles) For my simple job, it's easy enough for me to manually check the lead-ins and adjust if necessary. On more complex layouts, I'd expect that would be a much more daunting task.

[steve_g]

Ross

I had a similar problem with a lead-in clipping another part today... My problem turned out to be two separate toolpaths unaware of the others existence. Toolpath lead-in/out extensions are only aware of vectors selected at the same time. Any chance your situation is as simple as that?

SG

[Ross Leidy]

The two closed vectors each had their own independent profile toolpaths. Are you saying that what is considered "waste" when a lead-in is added only takes into account the selected vectors? (And all the other toolpaths in the file are ignored?)

[adrianm]

I don't use lead-ins myself but that's how the other toolpath operations work.

You have to make sure there is enough clearance between vectors with their own toolpaths yourself. The software doesn't look at other toolpaths.

You can set the solid option on the 2D toolpath preview to see where toolpaths might run into each other.

[Joe Porter]

The "Lead In" length is up to you...like Adrian said, I wouldn't use the Lead In option...joe

[steve_g]

In defense of lead-in/out...

I like to use lead-in/out for my toolpaths... not using them can result in slight blemishes where the bit goes down or up. Even using the spiral down option does not prevent a straight up retraction with the bit against the finished part. You don't need to use long leads... in fact very short ones are just fine. In Ross's situation, he's using a compression bit and needs a lead-in long enough to get the bit to final depth before cutting on the part...

SG

[Ross Leidy]

Thanks for all the comments, guys. Now that I know I need to look for an errant lead-in, I'll just incorporate that step into the process. Steve's point about a shorter lead-in will easily solve the problem for me. I don't need it to be long at all. I think 0.25" would be plenty.