Bevel Edges using VCarve Pro

[Keith Larrett]

I need to cut a bunch of panels from 3/4" MDF. They need to have a bevel edge such that the flat side of the cut is 1/4". I guess that means they will have a 1/2" bevel.

I'm trying to work out the most efficient cutting strategy. I'm using a 91 degree miter fold v bit (close enough to 90 degrees for the job). I first cut the outline of the panels with a 3/8" compression bit. Then I am running the v bit at a depth of 0.5625 and offset of 0.0625.

I have the profile path set to cut on the line and am cutting in two passes with the depth of the final pass being 0.125".

Is there a way in VCarve to do the final pass in the opposite direction when cutting on the line?

Would it be better to use the V Carve Toolpath and set it to a cut depth of 0.5" along the outline path with no offset?

I guess I'm trying to avoid cutting with the "point" of the bit by using the offset strategy.

I'm also cutting all the lines along the X Axis and then all the lines along the Y Axis as opposed to cutting out the rectangles individually. I'm assuming that would make for faster cut times with cleaner cuts as the machine is not turning any corners, just travelling in straight lines. Is that thinking correct?

I'd appreciate any advice!

[joe]

Not sure this is CNC work.
If this work came to my shop I'd use the panel saw and router table.

[Keith Larrett]

Thank you for the reply Joe. You're probably right, but I don't have a panel saw. I also lost all enthusiasm for cutting 4'x8' sheets of MDF on my Ridgid table saw the day my ShopBot arrived :)

[Kyle Stapleton]

What you have stated will work fine.
Not sure how to us the last pass (no Aspire 8)

I would run the v-bit before the profile to keep the parts in place but seeing you have a big vac doing it last should not hurt.

[bleeth]

Get a 45 degree bevel bit with a bearing and run the bevel with a hand router.
As far as reversing direction on the second cut just set up two toolpaths. First depth in conventional and second depth in climb.

[dlcw]

I do a LOT of sports plaques out of 1/2" MDF for a local company. They require a rounded over edge. I cut the plaques on the CNC, then round over the edges on the router table. Has worked well for me for about 6 years now.

[scottp55]

as far as changing direction on the last pass...you already have last pass selected...now just check the box for reverse direction?

[Keith Larrett]

Get a 45 degree bevel bit with a bearing and run the bevel with a hand router.
As far as reversing direction on the second cut just set up two toolpaths. First depth in conventional and second depth in climb.

Thank you! I didn't think of that, probably to obvious :)


as far as changing direction on the last pass...you already have last pass selected...now just check the box for reverse direction?

The section for reverse direction is "greyed out" and can't be selected. I guess it is only for cuts made inside or outside of the line, not for cuts made on the line.

I appreciate all the replies. I'm curious why there seems to be overwhelming consensus for running a hand held router with bearing bit or running the cut parts on the router table. What is the advantage of that over using the CNC to run the profile? Not trying to argue with the collective wisdom, just trying to learn. Thanks.

[RossMosh]

Thank you! I didn't think of that, probably to obvious :)

The section for reverse direction is "greyed out" and can't be selected. I guess it is only for cuts made inside or outside of the line, not for cuts made on the line.

I appreciate all the replies. I'm curious why there seems to be overwhelming consensus for running a hand held router with bearing bit or running the cut parts on the router table. What is the advantage of that over using the CNC to run the profile? Not trying to argue with the collective wisdom, just trying to learn. Thanks.

On straight cuts, you need to change the start point to change directions.

[joe]

To answer the question, why use an alternative bearing bit. Do a panel both ways and you'll see.
A CNC is substitute for a saw when you must. A good router table is a must for precision work.

[bleeth]

Bearing bit in a hand router is a h*ll of a lot quicker and easier. (IMHO)
No bit changes, programming time, etc. and it would do the whole thing in one pass like nothing.

[joe]

I usually do a second, "kiss cut" to give an ever so smooth finish. Not sure I have ever been able to top this with a CNC. It's so easy to build a little router table for this kind of work.http://www.talkshopbot.com/forum/attachment.php?attachmentid=26982&stc=1

[bobmoore]

If I was making a couple dozen of those I would follow Joe's suggestion. Many dozen and I would use the bot if your table is very flat. That way you can have a cup of your favorite coffee while the bot works. If I was cutting hundreds of them I would build a dedicated vacuum fixture from mdf and the allstar or similar tape. They make a consistent .030 thick by .5 wide that I use a lot. Get mine from my tool supplier because they are close however I am pretty sure they also sell direct.
Bob

[knight_toolworks]

when I do these on the machine I cut one direction but make the final pass .02 in depth that gives the accuracy right now I am doing these sheets of 3/4" so with a 90 on line 1.5 ips three passes the last pass is .02 cuts pretty well then. I don't have the room to cut large panels on my tablesaw.

[Keith Larrett]

Thanks again for all the responses. I did a test panel and was pleased with the result.

I decided to use the CNC for this as I have a number of panels to cut. I also anticipate cutting large quantities on a semi regular basis in the future, so it was worth the time to prepare the tool path.

[Cosmos275]

What I do is run the chamfer tool on the outside of the profile and use a negative offset. VCP behaves weird (imho) such that when you offset a v-bit, it will slide down the cutting edge, so you'll never get the bevel (it will always not cut into the profile). But, using a negative offset works. For a 0.5mm chamfer, I run 1.0 depth and -0.5 offset.

[Tim Lucas]

Thanks again for all the responses. I did a test panel and was pleased with the result.

I decided to use the CNC for this as I have a number of panels to cut. I also anticipate cutting large quantities on a semi regular basis in the future, so it was worth the time to prepare the tool path.

Looks like a good cut and I am with you, let the bot do it so I can repeat it often