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:

Regen times skyrocked suddenly.


Cygnus1
 Share

Recommended Posts

im running mastercam 2021 Working on an electronics encloseure. its a pretty complex part but nothing new. added a Surface high speed(Dynamis OptiRest) and its taking around 1.5 hours to regen. this is a pretty typical thing for me but its normally 1-2 minutes. oddly while regenerating there no load whatsoever on the cpu. Is there anything i can try to speed this up. any issues to look for. 

I cannot share the model or any pictures its ITAR work. Watching the Multithreading manger its the calulating step up and down that take all the time. using a 1/4 em step down is 150% stet up is 50%. max depth is .75" part overall is 12" x 18"

Im open to trying anything at this point. 

Computer Specs

cpu i9 9900

gpu quadro p1000

windows 10 pro

Link to comment
Share on other sites

I am using a boundry. and everything looks very typical in all the settings. I have been having issues with models from this customer. could it be a bad model. it looks and acts normal. I had issues with micro gaps in the model and surfaces being attached just weird stuff previously. The model was made in NX.

Link to comment
Share on other sites

One other thing you may wish to try is if your working over a network save the part locally and try regening it. Our network is good but we have some complex parts that when they start to take time crunching numbers we begin to work local and it helps a lot.

Just remember to save your part back to the network if that's your protocol 😃

Link to comment
Share on other sites

If the issue is with the operation, then u can chain any solid and use it as an example.

If you use the same toolpath on a simple solid, that should tell you something.

You could also just convert the solid to a mesh and drive the toolpath with that instead..

Link to comment
Share on other sites

I reported this as a bug in MC2021

A large solid model with 30/40 drilling ops was taking 9 minutes to regen when using solid geometry

The same file using wireframe regened in about 10 seconds

It has been fixed in MC2022. Wireframe is still faster but the solid drive file regens in about 45 seconds

I still notice a delay in solids driven surfacing and 5x paths, but it's manageable.

 

 

Link to comment
Share on other sites
35 minutes ago, Brad St. said:

Interesting Gcode, if you were to create surfs from the solid of only the geometry you need to process (I know not ideal) does it crunch differently?

Yes

I'm currently working on a part Ø127" by 15" tall

It looks like a 12 bladed star

I'm doing some basic high speed waterline toolpaths using the solid model as drive geometry

One path takes 15 to 20 seconds to regen

The identical toolpath, driven by surfaces regens instantly

  • Like 3
Link to comment
Share on other sites

The other thing to keep in mind when using Solids is this:

  • Mastercam has to process "every face" of the Solid, when you select the entire Solid Model. This includes all of the "hidden" faces. (Faces which are "below" some geometry that is above those lower faces.) This takes overhead to process.
  • It is more efficient for the toolpath to process if you manually select "only the visible faces" of the solid, rather than the entire solid model.
  • All of the "Opti" style paths, are making assumptions about "where is the 'Stock' that needs to be removed"?
  • Because of this issue with determining where the stock lies, these Opti Paths work best when you use some sort of Stock Model, to alert the path to where "stock really exists" in the real-world. The path has a much easier time crunching when it "knows where the stock is that needs to be removed". For stock, if you are using a Mesh Model, you need to pay close attention to the Tolerance used to generate that stock. The more "triangles" contained in the Mesh, the longer the processing time.
  • USE YOUR TOLERANCE for the Path!!!! < I can't tell you the number of Mastercam Programmers that I see, who never, ever, adjust the Cut Tolerance, and never enable the Line/Arc Filter. You should always be adjusting the Cut Tolerance for Roughing. Use 10-20% of your Stock to Leave value. If you are rouging, and leaving 2mm (0.08") of stock on your model, your Cut Tolerance should be 0.004-0.008 (0.005" would be good here), and your Total Tolerance could be 0.010-0.020". For roughing, I typically use a 1:1, 1:2, or 1:4 ratio, between Cut Tolerance, and Filter Tolerance. In my example, with 2mm stock (0.080"), I would probably run 0.010" Total Tolerance, with a 50/50% split (1:1), or a 0.020" Total Tolerance, with a 25/75% split. (0.005" Cut Tolerance + 0.015" Filter Tolerance.
  • Remember that the Tolerance is "bi-directional" or a (+- Tolerance. So if our offset is 0.080" from the part, and our Total Tolerance is 0.020", we could be leaving "as much as 0.100", or "as little as 0.060"! Typically, that +- stock amount isn't that extreme, but it also depends heavily on the shape of your CAD geometry, the Cut Pattern, and other factors. The most important setting is the "Cut Tolerance".
  • Like 2
Link to comment
Share on other sites
1 hour ago, altamontmfg said:

You mean machines from the 21st Century?? lol

You get used to modern convenience quickly. 5 years ago I was soldering an RS232 cable to drip feed to my first CNC machine- a used 1980s Okuma. A few weeks ago I had to use a Compact Flash card on a newer machine and it felt like the biggest bother of 2021 so far.

  • Haha 1
Link to comment
Share on other sites
18 minutes ago, Chally72 said:

You get used to modern convenience quickly. 5 years ago I was soldering an RS232 cable to drip feed to my first CNC machine- a used 1980s Okuma. A few weeks ago I had to use a Compact Flash card on a newer machine and it felt like the biggest bother of 2021 so far.

Agreed. I'm quite spoiled these days when it comes to equipment.

Link to comment
Share on other sites
1 hour ago, altamontmfg said:

You mean machines from the 21st Century?? lol

Serious Answer > I've had to use the Section NCI Chook to break up a single Roughing Toolpath into 80 Kb programs, and run them sequentially (and painfully) on the Control. For those with limited memory, DNC becomes a Godsend.

If you are in this situation; do yourself a favor and invest in a quality cable for the data transfer.

Predator Hardware makes an absolutely awesome kit, which uses a special "tripple shielded" Ethernet Cable as the link between host and machine. Predator makes adapter ends, which terminates in any of the common machine configurations. This makes the cable as plug-and-play as possible, while providing much better shielding. 

  • Like 4
Link to comment
Share on other sites
18 hours ago, Colin Gilchrist said:
  • USE YOUR TOLERANCE for the Path!!!! < I can't tell you the number of Mastercam Programmers that I see, who never, ever, adjust the Cut Tolerance, and never enable the Line/Arc Filter. You should always be adjusting the Cut Tolerance for Roughing. Use 10-20% of your Stock to Leave value. If you are rouging, and leaving 2mm (0.08") of stock on your model, your Cut Tolerance should be 0.004-0.008 (0.005" would be good here), and your Total Tolerance could be 0.010-0.020". For roughing, I typically use a 1:1, 1:2, or 1:4 ratio, between Cut Tolerance, and Filter Tolerance. In my example, with 2mm stock (0.080"), I would probably run 0.010" Total Tolerance, with a 50/50% split (1:1), or a 0.020" Total Tolerance, with a 25/75% split. (0.005" Cut Tolerance + 0.015" Filter Tolerance.
  • Remember that the Tolerance is "bi-directional" or a (+- Tolerance. So if our offset is 0.080" from the part, and our Total Tolerance is 0.020", we could be leaving "as much as 0.100", or "as little as 0.060"! Typically, that +- stock amount isn't that extreme, but it also depends heavily on the shape of your CAD geometry, the Cut Pattern, and other factors. The most important setting is the "Cut Tolerance".

Another interesting video about cut/filter/smooth tolerances in Mastercam.

Link to comment
Share on other sites

Many good things stated here.

 

Another one which may come off as beginner advice but is true, is to dial in a toolpath using a massive stepover to make sure everything looks correct with containment, collision control, etc. Lets say you want your final stepover to be 0.005" for a surfacing finish pass. Set your stepover to 0.050" or 0.1" and then when everything is dialed, you change the final stepover to 0.005". Helps save a lot of regen time when you just need to make sure the toolpath is going to work.

  • Like 1
Link to comment
Share on other sites
16 minutes ago, Metallic said:

Many good things stated here.

 

Another one which may come off as beginner advice but is true, is to dial in a toolpath using a massive stepover to make sure everything looks correct with containment, collision control, etc. Lets say you want your final stepover to be 0.005" for a surfacing finish pass. Set your stepover to 0.050" or 0.1" and then when everything is dialed, you change the final stepover to 0.005". Helps save a lot of regen time when you just need to make sure the toolpath is going to work.

A very good point that often goes overlooked. Also, if you're going to end up with a Spiral cut pattern choice on a multiaxis path, leave that set to one way or zigzag, and change it back to spiral along with the final stepover as the last changes you make to the path. Spiral is another choice that can drastically increase calculation time.

  • Like 1
Link to comment
Share on other sites
2 hours ago, Chally72 said:

A very good point that often goes overlooked. Also, if you're going to end up with a Spiral cut pattern choice on a multiaxis path, leave that set to one way or zigzag, and change it back to spiral along with the final stepover as the last changes you make to the path. Spiral is another choice that can drastically increase calculation time.

Yes, same story with Depth Cuts and/or Multi-Passes. Get your "cut pattern" working first, without any "extras", and then worry about adding things.

This is especially true with "Tool Axis Control" methods. Don't enable the Collision Control stuff, until the very end. Worry about "how does the tip of my tool look, as it traces over my surfaces. Don't worry about Tool Axis collisions, until after the cut pattern looks good. Once you get the cut pattern "dialed in", then you can start adding the Collision Control strategies, one-at-a-time. Don't "add them all at once". First, add your "Retract Tool Along Tool Axis", to your "Check surfaces". This typically gets you your "tool tip tangent to the surfaces you want to leave behind". Get that working first, then add "Tilt Tool" or another "avoidance" strategy.

Get in the habit of building your 5-Axis Paths "from the bottom up", rather than trying to figure out "what are the optimized setting for everything all-at-once.

Chase perfection in the following order:

  1. Cut Pattern > Loose Tolerance + large stepover. (make sure the "toolpath trace" is moving correctly.
  2. Set an "initial" Tool Axis Control Method.
  3. Add "Collision Control" (Retract along tool axis), so that the tool tip is now staying "tangent" to the surfaces you want to "leave behind". This could be your "Drive" surfaces, but more often than not, these are the "Check or Compensation" surfaces.
  4. Tweak Tool Axis Control Method if necessary.
  5. Add "additional Collision Control" if necessary. Many 5X Paths that I create only use the 1st CC option (retract along tool axis), and I don't need additional strategies. Remember > each additional strategy means your path must collision-check each vector position "again". This add calculation time.
  6. Adjust your Linking Options. (Add lead in/out moves, adjust Gap Settings, Etc.) Make sure the tool enters/exits how and where you want.
  7. Finally > set your Cut Tolerance and Step-over values to the final values. Enable Depth-Cuts and/or Multi-Passes, and let the calculations run, while you do something else.
  • Thanks 1
  • 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...