Custom tool failure

[pip]

I've got this alarm coming up when trying to produce a custom tool in tool manager mcx8. Any one able to help. Have checked the drawing far too many times. Inside the mcx8 file it works with no problems, but when I export the dxf, for importing into tool manager, I get this message..

[jlw™]

Can you post your dxf? Once you figure it out it's incredibly easy.

 

Do you have cut and nocut levels?

[Guest]

You need in a dxf to have at least 2 levels....

 

One named cut and the other named nocut

 

The tool geometry should be on the cut level....

 

if you choose to define a holder, that would go on the nocut level

 

Also, geometry for a dxf should be in the upper left quadrant X-,Y+

 

Which IS different the using a mastercam file which is X+,Y+

 

The dxf change is to bring it into compliance with the ISO standard

[Müřlıń®]

Too much work.....all I do is to build the tool on a level of my choosing and save it as a Mastercam file...

 

Then merge it into my working file and import to tool manager.

 

Need to edit the tool??   no problem....just open up the level and make changes.

 

That way all custom tools are in the file they are used for and don't come from a tool library...

 

You can use that tool in another file just merge it in and use it...

[Eric@HorsepowerInc.]

Too much work.....all I do is to build the tool on a level of my choosing and save it as a Mastercam file...

 

Then merge it into my working file and import to tool manager.

 

Need to edit the tool??   no problem....just open up the level and make changes.

 

That way all custom tools are in the file they are used for and don't come from a tool library...

 

You can use that tool in another file just merge it in and use it...

 

^^^agree

[Guest]

When you realize that's how your holders have to be done, you might not think it such a big deal...

 

Plus, when you get tool data from a vendor, that's the most likely format it will come in

 

Change fella's get on board or get run over  

[Eric@HorsepowerInc.]

When you realize that's how your holders have to be done, you might not think it such a big deal...

 

Plus, when you get tool data from a vendor, that's the most likely format it will come in

 

Change fella's get on board or get run over  

JP, curious why you say it like that? There's not a single thing I/we couldn't do in X2 that X9 or so on has enabled. On board or off, we sail our own ship..generally hate to follow. Has kept us going very very strong! At some point I think people think too far into this, at the days end it's those that put quality parts out the door the fastest wins.

[pip]

cheers guy. I will try that tomorrow at work.  JP you wrote that both the tool and holder are on the cut layer?  is this just a small mistake on your part or should the holder be on the nocut level.

[Guest]

Holder would be if included on the nocut level

[Guest]

JP, curious why you say it like that? There's not a single thing I/we couldn't do in X2 that X9 or so on has enabled. On board or off, we sail our own ship..generally hate to follow. Has kept us going very very strong! At some point I think people think too far into this, at the days end it's those that put quality parts out the door the fastest wins.

 

Just being a little facetious this morning is all  

 

[gcode]

something new in MC2017..

you can import step files to create both tools and holders

I've had excellent results with this using Sandvik Capto models

for tool holders

I download the sldprt files from Sandvik, mate them in Solidworks

export as step and create a accurate tool holder in Mastercam

with very little effort

I've also had pretty good results using Sandvik's step models of their ball insert mills

to make custom tools in MC2017

[crazy^millman]

 

something new in MC2017..

you can import step files to create both tools and holders

I've had excellent results with this using Sandvik Capto models

for tool holders

I download the step files from Sandvik, mate them in Solidworks

export as step and create a accurate tool holder in Mastercam

with very little effort

I've also had pretty good results using Sandvik's step models of their ball insert mills

to make custom tools in MC2017

 

 

The Dynamic Xform can mate them very quickly as well. I use it all the time with very good results for those that don't have a CAD system outside of Mastercam.

[Müřlıń®]

When you realize that's how your holders have to be done, you might not think it such a big deal...

 

Plus, when you get tool data from a vendor, that's the most likely format it will come in

 

Change fella's get on board or get run over  

I don't build my holders...I just pick them from a holder library save my assemblies to a library and just swap out tools and modify the holder that is already made...easy peezy and don't have to jack wiff any of that.  

 

I could care less that my holder doesn't match exactly...its kinda like stock recognition...just have to be close cause it just don't freaking matter...  your tool clearance settings and collision control make all that moot...its all clearance...

 

Length and basic dia is all that matters.....not the .01 step, the chamfer or radii...

 

There is no reason to run your tool that close to the part so a chip can marr the surface, or a slight calculation can cause a rub...

 

Now if it is something the customer wants that is another issue entirely..

[4VRGJ03]

Ok I figured this out. After 3 hours using every possible combination of geometry configuration.

 The idea is to create a custom tool using the only the Tool Manager Program and a DXF file. I have attached the Mastercam File which I used to create the DXF for eveyone's reference.

 The DXF MUST have the following attributes.

 1 – 2 levels must be created and named as CUT and NOCUT

2- The geometry must be created on the upper left hand quadrant on the default TOP plane and on the CUT level

3- The length of the tool will be along the X axis (X-) and the diameter of the tool must be along the Y-axis (Y+)

4 – The tip of the tool must be placed at the origin

5 – The profile of the tool must be closed by a center line (ie. axis of rotation at Y Zero)

Save the file as a DXF  and load the DXF file and voila! There is a reason to doing it from the Tool Manager and not the Mastercam Interface which would take a while to explain. If anyone wants me to explain it let me know.

 My question is….where in any documentation does Mastercam tell me that this is required?? I have searched endlessly and could not find the prerequisites to what is required for the DXF file. 

DRILL.mcam

[?Mark]

Here

[4VRGJ03]

I'm confused as why this wouldn't be included in the "Tool Manager Getting Started" guide? Mabey that section is missing from my guide or mabey I just completely missed that section.

[crazy^millman]

8 minutes ago, M4573RMZD said:

I'm confused as why this wouldn't be included in the "Tool Manager Getting Started" guide? Mabey that section is missing from my guide or mabey I just completely missed that section.

Good question shoot off an email to CNC Software and bring it to their attention.

[[email protected]]

Thank you M4573RMZD, I was in your same boat saving every config but luckily I looked here after my first 5 attempts. I was trying to make a corner rounder with a long pilot. I dont know why you cant add extra pilot length on the corner rounder tool wizard.

[JoshC]

Keep in mind there is more than one way to make a custom tool in mastercam. 

Note: im talking mill custom tools only, not lathe custom tools

1. The DXF method, (requiring us to follow ISO 13399 standards - like the cut/nocut levels people above described)

most difficult method in my opinion

2. a solid model of the tool (tool must be a closed solid body, aligned with The Z-axis of top plane, Saved as a Step file)

second easiest method in my opinion

3. A 2d tool (All geometry same attributes and level, no splines supported, Aligned with the Y axis from top Plane, No centerline, saved as a mastercam file)

easiest method in my opinion