Problem- Shaped tool

[jake_tb]

Hi guys.
I have several custom face mills mounted backwards on their arbors to do reverse chamfering. I have sketched these in the shaped tool section but the zero point of the tool is always on the front tip. I need it on the insert tip that is 30-40mm away from the end tip of the tool. Does anyone have any suggestions on how to move the zero point back up the tool so it can simulate in solid verification correctly?

Jake

[jess fuqua]

Just draw the tool the way it is then use your levels and modify offset to fudge it in.
I do it all the time with my double angle harvey tool.

[foxsquirrel]

I just fudge it in, it can be done correctly because tech support walked me through it one time and I just cannot remember how to do it. Their manual is a little skimpy in that area and hopefully someday they will make a video for the shaped tools.

[Brakeman Bob]

I have done it by using the "Delta Depth" field on the Levels page. Like Foxsquirrel, it was some time ago and I can't remember quite what I did.

What type of tool is your shape tool defined as? EG is it a TEE SLOT or an ENDMILL? I seem to remember that the tool definition had some bearing on the matter.

Good luck with it.

[Aussie_CNC]

I don't think this is currently possible.

Fudging the delta or profile depth values might make it look right in the simulation, but then you have to set them back for the gcode output to be correct, so not ideal

The shaped tool geometry is always moved into positive z space, so even if you pick your reference point in the correct position (setting point of tool), the shape is always broken down into it's sections with the tip being Z0.

I had a quick play with the STL shaped tool option, modelling a tool in SW, creating a co-ordinate system at the tool set point, and then exporting the tool as an STL in relation to that co-ordinate system and selecting the option "do not translate into positive space". The tool image in the preview window looks ok (even though it doesn't give any idea whether the Z is correct), but it is not shown in SolidVerify. ...might be a question for SC support, as I've not used this STL option before?

[jess fuqua]

I don't agree, if your using a double angle tool your going to do some math.
CAD CAM can't make all situations easy.
Sometimes the programmer has to just make things work.

[Aussie_CNC]

The whole point of CAD CAM is to make programming easy! I agree that no CAD CAM system currently makes every situation easy, but they're all getting better with each release, and the ability to shift the tool set point would be very useful!

Anyway, what is it you don't agree with?

We have two clear situations:
1. where the tool is set on the machine
2. where solidcam considers the tool set point

In this case, the correct decision (in my opinion) has been made to set the tool at it's cutting point, so you need to output the gcode to match (which means the simulation will be wrong).
As this is a reverse mounted face mill, are you saying the tool should be set (in the machine) to the head of the bolt that fastens it to the arbour??

[jess fuqua]

I do agree with both ways working.
I always make Z.0 the front of my tool and top of my part.
I use double angle Harvey chamfer tool to chamfer O-ring grooves on the mill.
The front of the tool is Z.0 the back is not.
When I do my chamfers all the numbers make perfect since top and bottom.I have examples of this if you would like to see.

[mattpatt]

I needed to so a slot with chamfered edges. I ground up a T-Slot tool and then drew this up in the shaped tools. Set the tool as normal and used a T-slot operation. Worked well.

If I then wanted to use this same tool for doing an underside chamfer I'd just use a profile strategy and offset the toolpath at a "delta depth" of whatever is needed. Give it a good lead in/out to clear the job. I don't think this is a problem.

I haven't done it but a normal chamfer type op with delta depth would probably be fine too.

There may not be the perfect operation or strategy to do this sort of thing, but in my opinion SC is very easy to cheat with if you think outside the box a little.

[Aussie_CNC]

I think we're missing the point here. The delta depth options are perfect for offsetting the tool to get the right cutting position, but only if you are setting the tool to the tip on the machine. As soon as you want to set the tool anywhere else, either the gcode output or the simulation will be wrong in SolidCAM.

[mattpatt]

I honestly don't know if there's a way to set it up as you want.

There's another job I do which involves chamfering the underside. I cant flip the job and do it as I'd have to make a fixture and it's all 3D surfaces on the top so it's have to be micron perfect, which it doesn't need to be. And it'll save a bunch of time and money just running it all in one setting.

So I just ground up a HSS bit held in a boring tool with a 45 degree topside edge. I'm setting Z off the bottom of the boring bar, not the cutting edge, but a little bit of measure before hand (diameter and distance from bottom of boring bar to cutting edge) got me in the ball park. Then gave it a bit extra on the delta depth for starters and then fiddled with the tool length offset until it was spot on. This was a simple profile operation with some offset.

[gabert]

I am not shure if this will work. but in your programming you can add a special offset in the z axis to take care of the tool nose to picture option. This could be done for each special shaped tool. Do the math offset only when that tool is selected.

GDG