Hi - cutting my first mould cavity with my V23 today. Stressful day! It went well for a while - then I had a few scary issues. Anyone else had these?

The toolpath appears to have a bigger path for the cutter than the radius of the set cutter. It looks twice as big as it should be........?

Even if I boundry the cavity - The sharp cavity edge sometimes shows an unwanted radius when verifying?

When I change the cutter size, and recompute the toolpath, often the toolpath stays the same?

I tried equidistant offset and slice planer and the same problem, tried reloading the v23 in repair - but the problems persists.

There seems multiple faults? Never had any of this with V21.

Any ideas?

Do all of those issues add up to something I am missing?

I have just tried a few things to try to expose the issue.

I created a new simple 3d cavity to see if it was my file that was corrupt or something. But the problems persist - too big a toolpath offset rad and the sharp cavity edge is radiused on verifying.

So I open the model file (iges) in V21 - correct toolpath radius and sharp edge is retained on verifying.

I do not have V23 but here are a few things you can try.

Check to see if your solid model is water tight.

Look for any Rogue Geometry in the area where the problem is.

Check your tolerance settings.

If your using a boundary make sure it is a complete chain and not broken.

You can also check to see if you have any geometry (solids, lines, or arcs) doubles.

The only other thing to check is the Surface Normals. Be sure they are all Pointing Outward.

If these don't work hopefully someone with V23 will pop in to lend a hand or mouse in this case.

Good luck:)

Thanks for your prompt support Toby D. I thought also I was missing something simple - You might not have seen my 2nd post - I produced a different simple solid and tried toolpaths on that - and some of the the same issues persist. But its fine in V21 - so .....I'll try some more tests to try to better identify the issues over the weekend.

post a sample so we can see what you are going.

You can setup the tool path to go from the center of the tool or the tip of the tool.

Maybe that is what you are seeing.

Center of tool screen shot:

http://i564.photobucket.com/albums/ss86/damjuice/sf1004.jpg

Tip of tool screen shot:

http://i564.photobucket.com/albums/ss86/damjuice/sf1005.jpg

When using a boundary the center of the tool goes to the boundary. So if you want to keep the tool inside of the shape you need to offset for the radius of the cutter.

Offset for Radius of cutter Screen Shot:

http://i564.photobucket.com/albums/ss86/damjuice/sf1006.jpg

Hey thanks for that Allen 123! For taking the time to post such a clear reply. This forum is such a life saver - especially for people who work alone in remote places!

I spent some more time trying to narrow down the issues I am having. Either I have missed a setting or it seems to me something is going wrong with the software as it loads the tool size. See the the attached screenshot. I have deliberately put the boundry beyond the cavity edge to expose what looks like the issues. If I convert from my metric (as you are probably imperial) the toolpath is based on cutter tip, the cutter ball bose offset curve going down from the cavity edge looks way bigger than it should be. The curve looks like what would be needed for a 3/4" ball nose - but I entered a 1/4". Also another issue is see the verify image. The cavity edge is rounded. If I open the same part and settings in v21 this does not happen. You would expect this if the top was set at a minus Z setting or something but I have checked that sort of thing many times.

Regarding entering cutter sizes. I take it it is normal practise to: after a toolpath is generated it can be re edited - and the cutter size etc set different. Then the toolpath can be regenerated. I assume that means the software clears the existing toolpath and generates and displays the new toolpath based on the new information. If I am correct in that assumption then it is not working. well, sometimes it updates, and other times it does not. If I change the tool size to a new toolsize over and over, entering twice each time, it is more likely to update the toolpath.

It seems as though the software is having trouble accepting the cutter diameter details?

I have tried reloading V23 in repair, is it worth trying uninstall and reinstall?

Sorry, my screenshot did not upload. This time I hope.

Couple of things to check:

1. If you're using Manual Tools, it may not be using your tool info. On occasion, it seems to default to a .500" dia. Try a System Tool of your dia. to see if that's better. I don't know if Bobcad is addressing this yet.

2. Keep in mind that all outside sharp corners will have radii equal to your XYZ Allowance. So if it's a large allowance for roughing you will large radii.
Although everything should clean up in verify when you run the finish passes.

When cutting cavities, I translate/copy the parting line up .01" to allow stock for finish grind. I've found that's the best no matter what software or machine.

Good luck,
moldmker

Hey thanks moldmker! You guys are really quick to respond! Much appreciated.

I reply to your perceptive points:

Yes I thought it might be a manual tool loading issue also - so I tried via sytem tools but it was no better.

I used no XYZ allowance in the above trial.

Interested in your moving up your parting line 0.010" thats 0.25mm - wow that quite a lot to grind off - have I got that right?

You copy the parting line up.....I think you are saying you move your part down...and leave the setting for top at Z 0 ? Or do you mean shift the x/y plane down?
Thats a good plan, I must do that also. Before this issue imerged I cut my first V23 cavity - was good but I noticed a small cut on the corner of my cavity of about aah in thou.....0.002 ish.( Not a critical depth so I can grind that off). But I see why you do that. I suppose it can be due to cutter errors, depth setting errors, software accuracy errors, run out errors etc.

Getting closer to the issue!

See the attached screenshot - I selected a 0.157" ball cutter but the toolpath kept coming up much bigger, . So I measured it and it is a 0.250" offset - yes thats a 1/2 " thats seems to be stuck in there - which I have never entered...

....
Interested in your moving up your parting line 0.010" thats 0.25mm - wow that quite a lot to grind off - have I got that right?

You copy the parting line up.....I think you are saying you move your part down...and leave the setting for top at Z 0 ? Or do you mean shift the x/y plane down?
Thats a good plan, I must do that also. Before this issue imerged I cut my first V23 cavity - was good but I noticed a small cut on the corner of my cavity of about aah in thou.....0.002 ish.( Not a critical depth so I can grind that off). But I see why you do that. I suppose it can be due to cutter errors, depth setting errors, software accuracy errors, run out errors etc.

Here's my procedure for mold cavities:

1. Import model from Solidworks.

2. Translate/rotate model so top of model is Z zero.

3. Unstitch parting line surface and translate/copy Z+.01"
( This amount is dependent on job. I use .01" for molds that get heat-treated and polished. My machine is an old VMC, so I need to allow for spindle growth and accel/deccel issues. When I ran a modern shop with EDMs, .005" was the norm. I will gladly trade the time to grind something just to get that nice crisp parting line.)

4. Increase Top of Part value by the amount of Z translation.

5. Create G-code
( I read the code to make sure that Zs are cutting the parting line at +.01")

6. At the machine, set all my tool lengths off the top of the part. Then either drop the Z fixture offset .01" or do a mass edit of the tools and increase by .01".

Being a one man shop, there are no communication errors with setup people. That can be a problem when you start adding/subtracting lengths.

Good luck,
moldmker

Situation update: It has just slowly got worse. Now toolpath will not compute at all. I tried uninstalling and reinstalling, virus scan etc, - no difference.
I have emailed Bobcad with the details - I have spent so much time over the last few days - I'll just leave it alone now till I hear from them. Thanks moldmker for your details - I will study this when I the software is back on board. Thanks for all your help.

Sounds like a partial install. The files downloaded from the BobCad updates site are only updates to the initial install. Make sure you have a "FULL" install from the original purchased disc, then run the latest update patch from the website to get to build "1326". Make sure your install is not from one of the "Demo Downloads". Remember, disc install, then update patch. :)

Many thanks BurrMan! Your a star!

I was using my disc to reinstall and repair - I assumed it was the latest build as I only received it a couple of weeks ago. But that patch seems to have done the trick.

Straight away I am getting sensible toolpath and verification.