Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Pitch in your little gems that make mcam life easier


jlw™
 Share

Recommended Posts

with mastercam 2021's new Bounding Box Auto Feature you can build a plane quickly and easily on a part that is orientated incorrectly using this new feature.

1. first use bounding box, select the part, set bounding box to AUTO (this will orientate the bounding box to the shape of the part even if the part is rotated into a funky angle)

2. Go to the advanced tab of the bounding box and choose create plane

 

check out and you have a quick and easy plane, orientated to the part properly unlike the results we sometimes can see with planes from solid face. I do find afterwards i need to rotated the plane 90 Degrees but its still quick and easy

  • Like 2
Link to comment
Share on other sites

My top tricks that helps me the most:
 

-levels,isolate basic wireframe or surface geometry to drive 5 axis Toolpaths

-Dynamic X form to align the part in space to any WCS of your choice

-saving STLs after OP1, loading the STL as OP2 stock in a different machine groups. Personally I don’t use stock models takes too long generating every change, I’ll use optirest if I need to pick out excess stock 

-Creating a tool library and holder library with your shops tools in the shop and named the mfg etc for common jobs

-translating toolpaths, export/import toolpath for future similar work

-add remove features of solids,

So many tricks and still learning.

  • Like 1
Link to comment
Share on other sites
On 9/1/2020 at 8:43 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

That is a really good idea and one I am surprised not already in the software. Why I like this forum. I am always learning from others. Thank you for sharing that I for one appreciate it. Do you mind if I make this a formal request on the Official Mastercam forum? 

  • Like 3
Link to comment
Share on other sites
On 9/1/2020 at 8:43 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

That is a really good idea and one I am surprised not already in the software. Why I like this forum. I am always learning from others. Thank you for sharing that I for one appreciate it. Do you mind if I make this a formal request on the Official Mastercam forum? 

  • Like 1
Link to comment
Share on other sites

Extend tool to infinity in the advanced 5 Axis Toolpath issues. I have a project I have been working on for 9 months. I am machining the ID of a large part taking a HSK 100 RAH and a Knuckle 5 Axis head to machine the inside of. I have been fighting and fighting to keep unwind motion inside the part controlled the Moduleworks toolpaths create when using a Cylinder as your your linking control. I was just using toolpath editor to remove these problems. Well I had noticed in other others turning of the default extends tool to infinity was checked. I turned it off those toolpaths were instantly better. I am having to make some changes to some of the previously programmed operations. I was dreading the Toolpath Editor process again to remove them. I was thinking about adding some crazy walls inside of the part to act as Avoidance. I have gone back and forth for 2 days on the best way to control this. I then looked and see it it is checked. I have maybe 6-8 hours fighting this trying to find a better way. I turned it off and the toolpath that was taking maybe 5-10 minutes each to process then processed in 2360ms. Not only that but my okay looking toolpath went to a very nice looking toolpath.

 

image.png

  • Thanks 1
  • Like 2
Link to comment
Share on other sites
1 hour ago, crazy^millman said:

Extend tool to infinity in the advanced 5 Axis Toolpath issues. I have a project I have been working on for 9 months. I am machining the ID of a large part taking a HSK 100 RAH and a Knuckle 5 Axis head to machine the inside of. I have been fighting and fighting to keep unwind motion inside the part controlled the Moduleworks toolpaths create when using a Cylinder as your your linking control. I was just using toolpath editor to remove these problems. Well I had noticed in other others turning of the default extends tool to infinity was checked. I turned it off those toolpaths were instantly better. I am having to make some changes to some of the previously programmed operations. I was dreading the Toolpath Editor process again to remove them. I was thinking about adding some crazy walls inside of the part to act as Avoidance. I have gone back and forth for 2 days on the best way to control this. I then looked and see it it is checked. I have maybe 6-8 hours fighting this trying to find a better way. I turned it off and the toolpath that was taking maybe 5-10 minutes each to process then processed in 2360ms. Not only that but my okay looking toolpath went to a very nice looking toolpath.

 

 

I've run into this a couple times myself. I find that selecting it for table/table machines, and deselecting it for head/head machines, gives the best results. I'm not sure why.

  • Like 2
Link to comment
Share on other sites

Flip step over and Angle in 5 axis Parallel toolpath to flip the start. I have some pockets that are mirrors of each other. I could come up with one toolpath to give me the motion I wanted so I had to break each pocket up in 4 toolpaths per pocket. I still am not comfortable with Transform Mirror and when I tried to use Transform Rotate around the top of the part with the 8 pocket section with mirror on each I couldn't label them the way I wanted and I couldn't control stupid unwinds. I am on TAPE 25 of this project and coming down to the final details to make this a really nice program and part. I have the pocket on the Left side and I want the start to align with the curved tapered wall I just finished. I was just dealing with the weird start on the previous tapes, but now we are in the finish TAPE and I get very picky about even these little things in my 5 Axis code. It was not hard letting it just RAPID feed from the Left wall the the start of the back wall inside of the part to the right side to start cutting, but I knew it could be better. It then dawned on me to slip the Machining Angle in Z from 0 to 180 and then Flip the Step over. Now the toolpath is starting on the left side after finishing the left wall. Nothing anyone would ever really see or maybe even notice, but to makes all the difference in the world to delivery the best program possible.

 

image.png

 

Link to comment
Share on other sites
On 9/5/2020 at 11:33 AM, So not a Guru said:

I've run into this a couple times myself. I find that selecting it for table/table machines, and deselecting it for head/head machines, gives the best results. I'm not sure why.

 

Extend Tool to Infinity should  most commonly be unchecked in undercut scenarios, head/head machines, slot mills, etc. Picture a wireframe silhouette boundary being made off of your tool, holder, shank, and shoulder, and then an extrusion being made of each of those individual silhouette boundaries out to infinity. That's what this checkbox is doing in the background. So if you're working on a table/table and not doing undercuts, it's no problem for the virtual tool/holder to extend to infinity as a giant cylinder through the shop ceiling. Do the same thing on a head/head machine, and that extend to infinity is now a wildly swinging cylinder as you traverse across your part, which may or may not come in contact with drive surfaces, check surfaces, etc, across the table from where you're actually cutting.

 

So, why is Extend to infinity turned on by default and how exactly does it work? Let's consider my poorly drawn scenario, where I'm cutting across a sphere and have a toe clamp I need to avoid:

Tool1.gif.6d3c7bdaad90976c2504bf47bdbf0cd5.gif

 

OK, no problem, I turn on a retract tool strategy against the flute, and I add the toe clamp as check surfaces:

 

Collision.gif.e2ec11fa8034d936b22063da59303a24.gif

 

If I have Extend Tool to Infinity ON, I will avoid the clamp. 

If I have Extend Tool to Infinity OFF, Mastercam will not see the collision and I will crash through the clamp with the tool. Why? Because I told Mastercam explicitly to check the flute of the tool against my check surfaces, and guess what? My flute never touched the toe clamp! But the shank did. So, what this is doing by having that checkbox ON is extending the tool profile in the spindle positive direction to check against any possible conflict I didn't even consider as a programmer, like so:

Tool2.gif.d8dacec839f25887df779c8a08ab7ac3.gif

 

This, however, would be a bad thing if we were using a slot mill to undercut, because it is extending the entire outer profile to infinity as seen below, and probably trimming away most of the toolpath:

Slot.gif.95c4b4e42b2e1f26bf22ec9f1c9d75ed.gif

 

Similarly with head/head machines if we get into the ID of a big cylindrical bore, what it's doing in the background is shooting that extension straight through the opposite wall of the cylinder you're cutting, and then of course that part of the path is trimmed away or retracted against or whatever your collision control strategy is set to do.

 

That toe clamp collision situation would be difficult for a new multiaxis user to understand or predict, and so the safe choice, particularly with table/table setups and regular ball tooling that comprise the bulk of multiaxis programming, is to leave that checkbox on. 

Once we know this, the helper picture we get when we click that checkbox makes a bit more sense:

 

Inifinity.gif.ec0a081c706bf9013497433645b18041.gif

  • Thanks 2
  • Like 3
Link to comment
Share on other sites

Using the new swarf as a morph between curves on surfaces. I have tired all kind of toolpaths on this really difficult area and finally took the new school swarf and used it to act like morph between 2 curves. Got nice motion and done make the change at the bottom in Method to zig zag and make sure your linking is set to follow surface on large and small gaps with no lead in/out.

image.png

image.png

  • Like 1
Link to comment
Share on other sites
17 hours ago, crazy^millman said:

Using the new swarf as a morph between curves on surfaces. I have tired all kind of toolpaths on this really difficult area and finally took the new school swarf and used it to act like morph between 2 curves. Got nice motion and done make the change at the bottom in Method to zig zag and make sure your linking is set to follow surface on large and small gaps with no lead in/out.

image.png

image.png

Sweet idea Ron. Am I correct in assuming that you used the 4 straight lines for axis control?

  • Like 1
Link to comment
Share on other sites
15 minutes ago, So not a Guru said:

Sweet idea Ron. Am I correct in assuming that you used the 4 straight lines for axis control?

No need for the lines, that was an odd shaped feature I cannot show and I made new surfaces to drive the toolpath and that is what you see. Problem I was having was the notch in the top surface and the edges feathering in to half edges along most of the radius on the edge. This is where I break out my modeling methods and make something to drive the toolpath exactly like I want. The issue was Morph was not having it originally or Parallel so I switched to swarf, but really didn't need one way cuts for this finishing operation since I am using a ball endmill. I had used this method in the past, but forgot all about it and then it dawned on me where the switch was. I thought it was worth sharing so here we are. 

  • Like 1
Link to comment
Share on other sites
  • 4 weeks later...
On 9/11/2020 at 7:25 PM, crazy^millman said:

Using the new swarf as a morph between curves on surfaces. I have tired all kind of toolpaths on this really difficult area and finally took the new school swarf and used it to act like morph between 2 curves. Got nice motion and done make the change at the bottom in Method to zig zag and make sure your linking is set to follow surface on large and small gaps with no lead in/out.

Ron, I tried this, but I must be doing it wrong, because the path cuts on either edge of the surfaces, without touching the actual surfaces.

https://www.dropbox.com/s/5seokgpvs1fqchf/Morph1.mcam?dl=0

Link to comment
Share on other sites
57 minutes ago, So not a Guru said:

Ron, I tried this, but I must be doing it wrong, because the path cuts on either edge of the surfaces, without touching the actual surfaces.

https://www.dropbox.com/s/5seokgpvs1fqchf/Morph1.mcam?dl=0

Zeke, not a good example of where I would use morph that to be would be one of situations where I might try model prep to create a nice solid edge to work from that is constant all the way verse the broken one it is. Then I would get a to size ball endmill and one pass it with a parallel to curve using the lower edge and one cut. Then in the roughing tell it depth of cuts 2 or 3 finish passes with some spacing to finish it off nicely. Morph is  great toolpath, but this one of those where out of the box on those surfaces not going to play nice.

Also the file only has 3 surface selected when I selected all the radius surfaces it was better, but could be perfect with some model prep work IMHO. I don't care if I cut some air in places if the overall end effect is a good motion and a nice looking part. I care about quality as much as I care about the fastest run time possible.

Here is the file back with the morph working, but you need to think about some limits to control too much swing on your machine. I use the cone process to a normal vector line I put on a different level. I changed the feed distance to 2" to make sure it was high enough to clear any possible issues with walls. I also uncheck damp not needed on this part. I also used feed rate control to make sure you were getting feed moves between each large gap event on the part with the irregular surfaces of the fillets.

Dropbox link

 

 

Link to comment
Share on other sites
55 minutes ago, crazy^millman said:

I might try model prep to create a nice solid edge to work from that is constant all the way verse the broken one it is.

I had no idea this was possible! I know very little about Model prep. I'm going to search for some help on this, it would make programming a LOT easier.

Unfortunately, this particular model is a sheet solid that isn't watertight, and the customer says it is all that is available, so the model prep probably won't be much good in this instance.

Link to comment
Share on other sites
10 minutes ago, So not a Guru said:

I had no idea this was possible! I know very little about Model prep. I'm going to search for some help on this, it would make programming a LOT easier.

Unfortunately, this particular model is a sheet solid that isn't watertight, and the customer says it is all that is available, so the model prep probably won't be much good in this instance.

No it might not be a good choice on this file, but we can never know what is possible until we try the impossibles in life.

I think you are on the right track and was able to make morph do better than what you originally had so might be good enough to help you get that area done and move on to the next thing.

  • Like 1
Link to comment
Share on other sites
Just now, crazy^millman said:

No it might not be a good choice on this file, but we can never know what is possible until we try the impossibles in life.

I think you are on the right track and was able to make morph do better than what you originally had so might be good enough to help you get that area done and move on to the next thing.

Yes sir, definitely helped. With the added bonus of getting me to look into the model prep capabilities.

Thanks again.

Link to comment
Share on other sites
18 minutes ago, So not a Guru said:

I'm going to search for some help on this, it would make programming a LOT easier.

Model Prep is great, Giang the tool had a youtube video that illustrates using thr push and pull, move functions, It's crazy powerful.

I had some parts that were drawn including the finish Material, about .020 " model prep push fixed them up real easy

Link to comment
Share on other sites
2 minutes ago, byte me said:

Model Prep is great, Giang the tool had a youtube video that illustrates using thr push and pull, move functions, It's crazy powerful.

I had some parts that were drawn including the finish Material, about .020 " model prep push fixed them up real easy

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.

I love Giang the the tool's videos.

Link to comment
Share on other sites
2 minutes ago, byte me said:

Model Prep is great, Giang the tool had a youtube video that illustrates using thr push and pull, move functions, It's crazy powerful.

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. 

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.   

  • Like 1
Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • 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

×
×
  • Create New...