Lead ins and

[andrewm]

I have a few part files now that we are running a lot of which has given me time to really watch what is going on. In a few of the parts I am noticing the when my bit plunges for the first cut that it is burning the material. It doesn't affect my final part, but I know its not good on the bit.

I am using Parts Wizard 2 and using the "Add Bridges to Start" option to hold my parts in place. I tried using the "lead in", and though this eliminated the burn on the part, the burn was still occuring on the lead in. The burn is occuring because the bit isn't moving forward in the material. Once it starts moving forward into the part, its then properly loaded and I am getting a good cut and the bit is cooling properly with the ejection. I have noticed that this happens the most when I use the add bridge function. Many of these parts could never be cut without the bridges. I don't have a vaccum table so I have to be clever about how things get cut and the bridges are a great feature.

Is there an easy technique to get the bit to plunge into the material as it is moving forward? Some quick coding technique verses going into the part file and manually calculating the moves?

I am cutting 3/4" MDF single pass.

Andrew

[paco]

Are you plunging fast enought... could you consider plunging faster (not too much though...)? Have you tryed/tested SB tabs (test'em in preview first since there are some issues regarding'em... should be fixed soon...)? Are you plunging passed the flute lenght? Are the bit long enought? About the "special codes"; others "Botters" could lead you through some "technics" that I don't know about... might want to consider a new CAD/CAM software...

[waynelocke]

You may be using a bit which is not a bottom cutting or plunge bit and with the lead in moves it is able to plunge.
Wayne locke

[paco]

Wayne is right! I would add that you could "manually" create a "peck plunge" strategie for your lead-in in PW...

[A McClary (Unregistered Guest)]

The bit is a downcut spiral so it is trapping the dust. We are using the downcut because we don't have a vacum table and I need the down force to keep some of the parts in place. If I do it in 2 passes I don't get this problem because the time the bit is in one place is shorter. Two passes takes too long. Plunge rate is .75 in/sec. We are trying to optimize this part file because we are cutting a lot of it each day.

My thought was to program a 3D lead in the beginning of each part so that the bit would move into the part gradually as it moves forward.

Adding something like this to the start of each part.
M3 3,3,0 'back up .75 inch from start
M3 3.3.75.-.75 'This is the start of the part.

Would this be worth the time?

The tabbing feature in SB doesn't put the tabs where they are needed. Nice feature, but doesn't work in my case. New software would be nice except PW2 gets me 95% of the way there. I can't justify thousands of dollars for a lot of features I wouldn't use.

[Brady Watson]

Andrew,
You seem to be on the right track with your ramping routine. That's where a little time and programming thought goes a long way. Is it possible to come into the material from the side @ full depth? How about making a circular profile move that steps down (effectively drilling a hole larger than your bit dia so it doesn't get trapped) and then moving right into the profile pass at full depth?

Just a thought...
-Brady

[paco]

Great idea Brady about cutting at hole at lead-in... Andrew; what about a straight bit?!

[beacon14]

If there aren't too many parts on the sheet, one option would be to change the Z parameter for the plunge of each lead-in to 0. Then, instead of a full-depth plunge, with burn, the bit would plunge only to the work surface, then (assuming the next move is a M3) the lead-in would plunge from Z=0 to Z=full-depth simultaneously with the X/Y move, ending at full depth at the edge of the part.
Did that make any sense? Not automated, but if there aren't too many parts on the sheet and you will be running the file many times, it would be worth the time to do manually

[andrewm]

David, I think what you are thinking is along the same lines as mine, but I was going to back up a bit to take the run into the plunge.

I used to use single flute straight bits till I was introduced to the Onsrud downspiral chipbreaker bit. (60-950?) They were recommended by the Onsrud rep when I was at the big wood furniture show a few months ago. Cuts through MDF quickly and gives a much cleaner cut which requires less finishing. The onther nice side effect is that the noise is about 1/3 of the straight bit. But since they aren't cheap I am paying a little more attention to my cut files than before. My whole reason for asking this is not because of the burn on my MDF, but I know the burn on the bit does nothing but dull it faster.

I like the idea of a little circle moving down, but not sure how that would be programmed easily.

I was thinking of trying to write a little VB program that would go through the file and look for the start of each part and then backtrack along the line of the cut .75", then move forward into the cut arriving at full depth at the start of the file.

[elcruisr]

This is one of the reasons we switched to ArtCam Insignia. You can automaticly do curved or straight ramped lead in moves, which dramaticly extended the life of our tooling. The ability to have full control over tabbing placement meant more parts to the sheet with tighter nesting. You need this with small parts even with a vacuum hold down system.

A downspiral tool really needs a ramped entry as it is not a true mortising tool. If the part is repetitive than programming it in yourself would be worth the effort. But the ability to do this for every single run, no matter how small, is a big bonus. It's also alot easier on the motor bearings (especially if you run a spindle). We even find mortising tools do much better when ramped into a cut instead of a straight plunge.

I did my fair share of grumbling about the price but it's been worth it for us to upgrade software. The formula may tip the other way for other shops but I'd want to find a way to avoid a straight plunge with a downspiral tool.

Eric

[richards]

Using PartWizard and a little file manipulation gives me the ramps that I need. Here a code sample of a simple 12X12 inch square that shows the original file and the file modified to include a ramp. Note that the start point is in the middle of a straight line portion instead of starting at a corner.

' file to cut a 12X12 square
' 1/4-inch cutter
'
' code without ramping
'
J3,6,-0.125,0.30

[waltie]

Can someone tell me how to access the "bridge" feature in Part Wizard?

Thanks for your help