Too large a cut file?

Post by **edcoleman** » Sat Sep 02, 2006 2:05 am

OK, I've got something that I think is not quite right with a file I'm working on. I've got some text wrapped around a circle and I want to clear the area around the text (leaving the letters raised). I'm using a carving strategy with a 45 degree bit cutting down to 1/4" and then doing a pocket clear for the remaining area.

When I calculate the toolpath there seems to be excessive top to bottom jogs causing the cut file time estimate to be larger than what I think it needs to be (2-1/2 hours). I've done this sort of thing before and I know it will result in the carving I'm looking for and I don't even mind the time, but I would sure like to be more efficient (if possible). Am I doing something wrong in my toolpathing to cause what seems to me to be excessive "jogs".

thanks for any feedback guys....

-Ed

PS: I've attached a screenshot of the toolpath as well as the *.crv file. However in the *.crv file I've removed the toolpath since it caused the file size to grow to about 4 Megs. Info on the toolpath: V carve with 45 degree bit, flat clearance with a 1/4" end mill. V carving speeds: 0.5"per sec plunge and move. Area clear speeds: 0.7"per sec move, 0.5" per sec plunge.

Post by **Jeff Guinn** » Sat Sep 02, 2006 4:48 am

Ed,
Usually this is a problem caused by the order used to select the vectors. Ungroup the individual letters,select each one in order starting with lower left corner & lastly select the inner & outter circle vectors. Apply your toolpath strategy & compare machine times. Hope this helps.

Jeff G

Post by **Paco** » Sat Sep 02, 2006 2:17 pm

I can't tell from your CRV file since there's no calculated toolpath in it but looking at the first image, I'd bet your stepover is very (too) small for either the end mill and/or V bit. It's even more difficult to tell since both toolpath are displayed so if you have there a 1/16 end mill with say 0.03" stepover for both bits, that can be a long term project... even in HDU foam...

Small stepover for cleaning up with a V bit make sense but do plan time ahead if you really want it...

As for the calculated time, make sure you got some relevant value there; rapids speed and scale factor (1.5-2 should give a rough average while 1 will lie to you not considering ramping up and down the feed speed).

PS: I'm mainly French and checking up spelling, it keep on telling me that stepover should be step over, stepdown should be step down, toolpath should be tool path even spoilboard should be spoil board and such; what right from wrong?!... in most CAD/CAM those words are a single words rather than two. Is my spell check (ThunderBird or Open Office) too fussy?!

Post by **edcoleman** » Sat Sep 02, 2006 3:05 pm

Jeff:

Thanks for the tip, I tried it and it did not seem to make a difference.

Paco:

I don't think that the issue is with the stepover (see the attached pics for info) but rather it is the fact that there are many jogs from the top to the bottom of the work piece. (I could post the entire *.crv file, but it is almost 4 megs and I don't want to clog up the board if it not necessary)

-Ed

Post by **edcoleman** » Sat Sep 02, 2006 3:22 pm

Paco:

In thinking about your response some more, I realized that I wasn't considering the "clearing" aspect of the vee bit. I'm used to simply vee carving the letters and allowing the bit to plunge as far as necessary to create the letter. In this project, I'm clearing around the letters but I'm limiting the depth of cut to 1/4". This is resulting in the vee bit going back and forth to clear areas that are too small for the end mill (see the attached file). I had thought that the top to bottom jogs were causing me the problem, when it was this area clear with the 45 degree vee bit.

I think that the bottom line is: with the constraints of this project the cutting times that I have are about the best I can expect.

Thanks again for the feedback !

-Ed

Post by **Paco** » Sat Sep 02, 2006 3:36 pm

edcoleman wrote:Paco:

In this project, I'm clearing around the letters but I'm limiting the depth of cut to 1/4". This is resulting in the vee bit going back and forth to clear areas that are too small for the end mill (see the attached file). I had thought that the top to bottom jogs were causing me the problem, when it was this area clear with the 45 degree vee bit.

I think that the bottom line is: with the constraints of this project the cutting times that I have are about the best I can expect.

-Ed

Number of plunges and retracts are directly related to the stepdown and stepover settings.

I would suggest (recommend) to clear as much as possible the flat with the end mill instead of the V bit as the end mill will make a bettr job at it... and may very well do it faster. Have you tried a smaller end mill step over?... have you considered using a 1/8" CED instead.
The bit bit will most certainly leave traces of material and tool marks; even in HDU and even more in woods and worst in non ferous metals.

BTW, most of the job time will be waste on V bit stepover rather than plunges and retracts... unless your tool is VERY slow.

Still, I yet do not know into what kind of material you'll be making this project... unless I've missed it?!

Post by **edcoleman** » Sat Sep 02, 2006 5:12 pm

Paco:

I realize now what you were trying to tell me regarding V bit stepover - that was the main issue with the large toolpath.

Also, I was clearing with a 1/4" end mill. Switching to a 1/8" helped alot, and after you mentioned it I hit myself in the head several times for not thinking of it myself

thanks for the help.

-Ed

PS: I neglected to mention that the material is HDU (my first project using this, I typically cut wood)

Post by **Paco** » Sat Sep 02, 2006 5:37 pm

The 1/8" CED may add a tool change considering the cutout but if your not in a hurry, it may still save you time at the end. To save on tool change on a such situation, I use a 1-1/8" CEL 1/8" CED foam cutting bit.
In fact, the very little material left from the 1/8" CED (inside details of your design) can easily be remove by hand or with a 0.02-0.03" V bit stepover. If I remember well, in your V bit toll setting you've posted, it was set to around 0.003" which would be good for plastics and non-ferrous metals.

HDU is probably the one material that will be clean the best with a V bit; with woods and others, you need to set the stepover to very small... or sand/polish.

Post by **Jeff Guinn** » Sat Sep 02, 2006 8:12 pm

When I calculate the toolpath there seems to be excessive top to bottom jogs causing the cut file time estimate to be larger than what I think it needs to be (2-1/2 hours). I've done this sort of thing before and I know it will result in the carving I'm looking for and I don't even mind the time, but I would sure like to be more efficient (if possible). Am I doing something wrong in my toolpathing to cause what seems to me to be excessive "jogs".

Ed,
Sorry, I misunderstood your original problem;thinking that repeated jogs from 1 side of your design to the other & back, rather than sequential cutting of toolpath for each bit, was your concern.
I agree 100% with Paco! Make sure your tool library has correct parameters & compare times using different diameter straight bits in combination with the same V bit.

Jeff G