Multiple tools for 2D Profile Toolpath?

[Onetrack]

Hi all, sorry if this is a basic question, but I'd like to run multiple tools when "cutting outside" using a 2D Profile Toolpath, however VCarve Pro v10.515 does not offer this. "Multiple tools" only seems to work for Pocketing Toolpaths. Is that right and if so, why, since it seems a bit strange! Thank you.

[Adrian]

Why would you want to do that? I can't think of a circumstance where it would be needed so it would seem strange to me if it was there rather than not.

[Onetrack]

I'm trying to cut out this gear, but the tool (1/8") is too large for the toolpath. I don't want to use a smaller tool (1/16") to cut out the whole thing since it would likely be a very slow operation.

[TReischl]

You are still going to have to use the 1/16 tool.

The worst part of it is that the 1/16 tool is still going to cut full width no matter what you do.

It is what it is.

I do not see any advantage to what you would like to see the software do. :::::shrug:::::

All that said, you could define separate toolpaths for the 1/16 tool and rough out with the 1/8 leaving, followed by a clean up pass with the 1/16th. No matter how you cut the mustard this is not going to be fast.

[Onetrack]

Thanks yes I realise I will have to use the 1/16" tool. However, I'm cutting lots to parts out and I'd like to minimise the time using the 1/16" tool. I think your suggestion is the best option, thanks.

[Adrian]

It's possible. There's just no one-click way of doing it. You'll have to create the vectors, setup two toolpaths . Getting a smooth finish with no stepping could be difficult given the different pass depths and possible bit deflection with a bit that small.

[Onetrack]

Its a shame you can't use nested toolpaths.

[TReischl]

I don't think you are going to save much time futzing around with two tools, developing paths, trying to get them nice and smooth, etc. Might waste more time trying to save time than you actually end up saving.

[adze_cnc]

I do similar things like this quite often.

• first toolpath cut almost all the way through the material (e.g. material thickness less your tab thickness) with an "allowance offset" of a small amount ( 0.006 inch say). This will be sheared off by the second bit
• second toolpath cut all the way thorough the material

The second toolpath's bit can often have a larger stepdown than usual as for the most part it is just shearing off the "allowance offset" above and it's going into small corners where there is less material to cut away.

[FixitMike]

To further expand on Adrian's post:
You can do a hack version of rest machining so the 1/16” tool will clean up only where the 1/8” tool won’t reach.
1. Offset the vector to be cut outward about 1/4”, or more if necessary to remove areas that can’t be reached by a 1/8” cutter cutting on the inside.
2. Add a virtual end mill .002” diameter to your tool list. It can have a pass depth equal to the total profile depth, and a 50% stepover. It won’t actually be used.
3. Select the original vector and the offset vector for a pocket toolpath cut. For this pocket toolpath use 3 tools, the .002”, 1/16”, and 1/8”. Be sure to include some (3D) tabs so the part doesn't move between toolpaths. Calculate.
4. Select original vector and calculate a Profile toolpath outside using the 1/8” tool.
5. Cut the Profile Toolpath.
6. Cut the 1/16” pocket toolpath. (Clear2) This should clean up the areas the 1/8” tool can’t reach. Do not use the .002” or 1/8” pocket toolpaths.
How this works: First, the profile toolpath cuts most of the periphery. Then, for the pocket toolpath, when more than one tool is used, the last cleanup cut includes the smallest tool running around all the edges to clean up any marks left by the larger tools. This will be what the .002” diameter tool does. It is included in the toolpath list so the 1/16” diameter does not waste time cleaning up the entire periphery, but it is not actually used. The 1/16” diameter toolpath leaves a small amount for this cleanup, but it will be less than .001”.
An example:

Rest machining example.crv

(241.5 KiB) Downloaded 53 times

[Onetrack]

I might try this...
I've added a circle and then placed vectors to cut around that circle, using a 1/16" profile cut.

cut times
1/8 (3.18mm) 18s
1/6 (1.59mm) 1.53s

worth a try!

[Onetrack]

Thanks adze_cnc and thanks Mike for the file, I will take a look at both methods...!

[TReischl]

Curious Mike? Since I do not have the latest version I cannot load the file and am way too lazy to duplicate what you did. . . . How do the cut times compare to just cutting it out with the 1/16th end mill?

Also, if there is not an auto tool changer then changing tools and re zeroing need to be factored in.

BTW, that is a pretty slick technique!

[FixitMike]

Curious Mike? Since I do not have the latest version I cannot load the file and am way too lazy to duplicate what you did. . . . How do the cut times compare to just cutting it out with the 1/16th end mill?

Also, if there is not an auto tool changer then changing tools and re zeroing need to be factored in.

BTW, that is a pretty slick technique!

The cutting time improvement depends entirely on the details of the part. The longer the profile distance, the greater the savings.
OP wants to use 2 tools. Using only the smallest takes too much time. He also said there were a lot of parts to be cut. I'm assuming he will cut multiple parts with each setup, so that tool change time per part is less.
Version 9.5 file:

Rest machining example 9.crv

(242 KiB) Downloaded 41 times

[TReischl]

The cutting time improvement depends entirely on the details of the part. The longer the profile distance, the greater the savings.
OP wants to use 2 tools. Using only the smallest takes too much time. He also said there were a lot of parts to be cut. I'm assuming he will cut multiple parts with each setup, so that tool change time per part is less.
Version 9.5 file:Rest machining example 9.crv

Ooops, that is a no go Mike:

Well, maybe I will fool around with it a bit this afternoon while the Turkey is cooking. . . .