jlw™

Pitch in your little gems that make mcam life easier

Recommended Posts

Guest
5 minutes ago, So not a Guru said:

I love Giang the the tool's videos.

Yeah, his videos helped a lot early on, very good content.

5 minutes ago, So not a Guru said:

Yep, I'm going to checking it out tonight. It won't do me any good on this job, but it'll be another tool in the pouch.

if you are allocating stock on a feature, you can use verify -> compare more effectively, than it you use stock to leave,

It's also more efficient for the toolpath..

 

Share this post


Link to post
Share on other sites
7 minutes ago, jerms said:

Model Prep is a great tool for imported bodies. I hardly ever use it on parts created in Mastercam. It deletes mastercam's solid part history. You will no longer be able to suppress features to create geometry from the model if needed.

I use it all the time on solids created in Mastercam. I copy the solid to a new level remove the history and make the changes from there. I have the original solid and the modified solid like I want. I just needed to make up some solid Mirco-100 lathe tools for MT to help get simulation dialed in. I made the Mastercam solids up to a point and the model prep to finish them up. Power of wireframe and solids all rolled into one without the 5X to 20X cost others are asking for about the same abilities. Not a parametric CAD, but when you understand the process you can work and do just about anything you needed. 

  • Like 3

Share this post


Link to post
Share on other sites
Guest
3 minutes ago, jerms said:

As for solid surfaces, it is important that the surface mesh is aligned. 90% of the time I will recreate net surfaces from solid edges. This makes morph and flowline tool paths much happier.   

Mastercam is great at creating complex net surfaces.

 

4 minutes ago, jerms said:

Model Prep is a great tool for imported bodies. I hardly ever use it on parts created in Mastercam. It deletes mastercam's solid part history. You will no longer be able to suppress features to create geometry from the model if needed

I usually clear the history, I don't do anything complex though, just the usual jigs and fixtures. Model prep lets me easily relocate pin alignment holes for positioning, since we do a lot of assemblies. 

Share this post


Link to post
Share on other sites

I just stumbled upon a useful hotkey that I was unaware of: When using Dynamic Move I accidentally hit my select all hotkey and noticed that when in dynamic move [Ctrl]+A toggles between part and gnomon movement so I no longer need to mouse click the icon located to the lower left of the gnomon to toggle.

  • Like 3

Share this post


Link to post
Share on other sites
15 minutes ago, Steelab said:

I just stumbled upon a useful hotkey that I was unaware of: When using Dynamic Move I accidentally hit my select all hotkey and noticed that when in dynamic move [Ctrl]+A toggles between part and gnomon movement so I no longer need to mouse click the icon located to the lower left of the gnomon to toggle.

The Control key is actually the hotkey that toggles this behavior- no need for the A.

This was a lightbulb moment for me when I discovered it as well. I use Dynamic transform for everything.

  • Thanks 1
  • Like 2

Share this post


Link to post
Share on other sites

Small Drills with Tapers between shank and drill are not definable in Mastercam.  Why this simple thing is so hard escapes me, but there is a way around it to get 100% accurate definition for CAV and even very when even .001" (0.0254mm) difference can scrap a part. Define the drill as the smallest diameter you are drilling. Then in the holder add the taper and shank of the drill in there and now you have correctly defined the drill, taper and shank. Here is a 1.5mm (.059") pilot drill and the next tool used will be a 1.5mm (.059") diameter 20X drill. Both were defined the same exact way with the 3mm shank down to the 1.5mm (.059") diameter with a 2mm taper length.

image.png.713ced2635b03204ebc4180768e25a6b.pngimage.png.16f1648dcf1f66a283b3f676c6b7fb77.png

image.png

image.png

 

  • Like 2

Share this post


Link to post
Share on other sites
20 minutes ago, crazy^millman said:

Small Drills with Tapers between shank and drill are not definable in Mastercam.  Why this simple thing is so hard escapes me, but there is a way around it to get 100% accurate definition for CAV and even very when even .001" (0.0254mm) difference can scrap a part. Define the drill as the smallest diameter you are drilling. Then in the holder add the taper and shank of the drill in there and now you have correctly defined the drill, taper and shank. Here is a 1.5mm (.059") pilot drill and the next tool used will be a 1.5mm (.059") diameter 20X drill. Both were defined the same exact way with the 3mm shank down to the 1.5mm (.059") diameter with a 2mm taper length.

image.png.713ced2635b03204ebc4180768e25a6b.pngimage.png.16f1648dcf1f66a283b3f676c6b7fb77.png

image.png

image.png

 

Yep, I've used this little hack for several things over the years. Can't remember off the top of my head what toolpath it was, but it wouldn't let me use a tapered ballmill, so I used this hack and used a regular ball in the toolholder.

Share this post


Link to post
Share on other sites

This was addressed in Ticket #28735-214797 for enhancements, specifically R-22884 not sure if it will be in upcoming release.

  • Like 1

Share this post


Link to post
Share on other sites
On 1/7/2021 at 10:24 AM, bd41612 said:

This was addressed in Ticket #28735-214797 for enhancements, specifically R-22884 not sure if it will be in upcoming release.

Well previous version will not have it do if someone needs it for that or right now it allows them to do what they need. :thumbup:

Share this post


Link to post
Share on other sites

Adjusting 5 Axis vectors for toolpaths can be a task. I have shared any different methods on this thread over the years. Jacob Ladder, back plotting toolpaths with certain lag and lead angles to get starts, end and edges for creation of vectors to drive 5 axis toolpaths. A new method that is proving helpful is 4 extents Vectors. I am machining the ID of a Large Cylinder using a Knuckle 5 axis head. Not full C axis as it is limited to +200/-200 of travel. Along the walls I have some ribs not normal to the ID and make putting the 500 lb gorilla of head into the 5lb space extremely difficult. I broken up what was one surface into 6 different surfaces and what was one toolpath into 4 different toolpaths. I used the my 4 vectors tweaking them until I got the motion I needed to keep the head from slamming the back of it into the other side of the ID, but also keep the tool from shanking out on the part. Trick was how to tweak these 4 different vectors at different angles real easy? Xfrom/Dynamic and the use the Gnomon adjust alignment switch to adjust Z to align to the Vector. Switch back to adjust and now I can move each vector the 2-5 degrees I need to see what happens.

I have a floor surface with some crazy features and transitions I made one toolpath for. Problem was what looks good in Mastercam was gouging the crashing in certain places in CAV. I had to break it up into 32 different toolpaths and trim and remake some drive surfaces to get good motion, but what it takes sometimes.

Share this post


Link to post
Share on other sites

Powersurface tip.

I have an area across some cross holes I need to machine. I didn't want the break dance process where I grabbed the surfaces around the hole and then had it jumping across to the next surface. I spent time trying to get Model Prep to remove the holes and the shape was just to complex. Spaceclaim couldn't handle it either. I made up a bunch of surfaces, but problem is they are surfaces and the toolpath is not nice and clean. I am getting little studders in the motion. Running a 5 Axis tool that is 18" gauge length with studders is not a good thing. I wanted a good surface and fought to better part of the day getting something. I finally got a good chain network to make a Powersurface, but the problem was it was not smooth towards the end of the shape and it was wrapping to close to the edge. I extended the cross chains .25 past the tear drop shape and then redid the Powersurface and now it fits into the area perfectly. Powersurface is a awesome tool and when we give it a little help it will do exactly what we need.

image.png.0c5403ba617fa89c69394896a5012286.png

  • Like 4

Share this post


Link to post
Share on other sites

Russian Roulette for Toolpaths. I have a tricky part where I need to mill what was going to be turned. Long story, but I need to take a lollipop cutter and use it inside of a bottle bore on the part. Gage length is 13.8" or 350.5mm and this is a nutating head machine. I got real good motion until about the 8th cut and then the parallel toolpath started jumping at the end from one edge to the other. It was enough to cause the machine to go into a over travel state on the B axis. I tired several different things through out the day trying to get it to quit. Then I remembered the old Russian Roulette method. Keep changing the step over until it quits. Now all 13 toolpaths stay engaged from top to bottom and life is good again.

  • Like 2

Share this post


Link to post
Share on other sites
On 1/16/2021 at 3:53 PM, crazy^millman said:

Powersurface tip.

I have an area across some cross holes I need to machine. I didn't want the break dance process where I grabbed the surfaces around the hole and then had it jumping across to the next surface. I spent time trying to get Model Prep to remove the holes and the shape was just to complex. Spaceclaim couldn't handle it either. I made up a bunch of surfaces, but problem is they are surfaces and the toolpath is not nice and clean. I am getting little studders in the motion. Running a 5 Axis tool that is 18" gauge length with studders is not a good thing. I wanted a good surface and fought to better part of the day getting something. I finally got a good chain network to make a Powersurface, but the problem was it was not smooth towards the end of the shape and it was wrapping to close to the edge. I extended the cross chains .25 past the tear drop shape and then redid the Powersurface and now it fits into the area perfectly. Powersurface is a awesome tool and when we give it a little help it will do exactly what we need.

image.png.0c5403ba617fa89c69394896a5012286.png

Be sure to check out the Overflow UV tool in 2022 to do similar things as what you've done here with PowerSurface without the same 3D input chain complexity! You might even see a Signature Parts video on it...

  • Like 2

Share this post


Link to post
Share on other sites
On 9/1/2020 at 11:43 AM, tpreb6 said:

I added all my common stock in the Geometry page on the HST so I don't have to keep changing or adding Stock amounts.

geometrysettings.jpg.6d475aae47daaa0b4dbd0d5944d7c5de.jpg

To do this, will I need to go into each individual toolpath and change it?  Or is there a way to do a mass change?

  • Like 1

Share this post


Link to post
Share on other sites
On 3/8/2021 at 10:16 AM, JB7280 said:

To do this, will I need to go into each individual toolpath and change it?  Or is there a way to do a mass change?

In 2022 you can copy machining and avoidance geometry groups and tolerances by right-clicking and dragging from the geometry dropdown of one toolpath to another toolpath or group of selected toolpaths in the operations manager. In this way, if you open your Operation defaults file and edit one operation, you could then drag these groups down to all the other 3D operations you might want these groupings on.

  • Like 2

Share this post


Link to post
Share on other sites

Negative cutting in the Moduleworks toolpaths. I make a copy of my tool and then change it to a smaller diameter tool. I want IT to cut .002 under all the way around a feature I make the the tool .001 smaller and then use it. I click on the don't output a tool change for the same tool number and have negative cutting on these toolpaths that don't allow a negative value. Note this is a 3D comp not a one direction comp. This will make the walls and floors a tool is cutting smaller.

  • Like 1

Share this post


Link to post
Share on other sites
On 11/2/2015 at 8:56 AM, jlw™ said:

No, for creating geometry.  For example, if you want to create a point a certain distance from another point I would create a point there then translate it.  If you shift-click you can type in X,Y,Z coords to put the point where you want it from the one click.  Try it with drawing lines or anything I've tried so far has worked.

Oh yeah I forgot about that one!

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now

  • Recently Browsing   0 members

    No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us